DriveWorks Solo Training

Design Automation
for SOLIDWORKS
SOL.V20

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DriveWorks Solo Training Overview

This training manual is intended to give a hands-on proficiency of DriveWorks Solo.

Upon successful completion you will be able to:

• Drive a SOLIDWORKS part and assembly geometry with DriveWorks Solo.

• Create DriveWorks Solo user forms and link them to the models.

• Control SOLIDWORKS Drawings.

• Create custom documents controlled by user inputs.

About this Manual

This manual is split up into a number of lessons.

Concepts
This covers the concepts of DriveWorks Solo, including best practice advice and tips.

The Concepts section can also be used post-training as a reference.

Concept:

Concepts are formatted like this.

Note:

Notes are formatted like this.

Tip:

Tips are formatted like this.

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Exercise
There is an exercise for each lesson. The exercises all work on the same models.

1. Exercise instructions are formatted like this.

Note:

Jumping between different exercises is not recommended as there is a flow of implementation

from one lesson to the next.

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Contents
DriveWorks Solo Training Overview ................................................................................................... 3
About this Manual .............................................................................................................................. 3
Imagine you design Wooden Doors .................................................................................................... 7
Lesson 1................................................................................................................................................... 9
Basic Setup.................................................................................................................................... 11
Opening DriveWorks Solo ............................................................................................................. 11
Creating a Project.......................................................................................................................... 12
Capturing your Models ..................................................................................................................... 14
Captured Assembly Structure ....................................................................................................... 15
Capturing Individual Models ......................................................................................................... 16
Lesson 2................................................................................................................................................. 31
Project Designer ................................................................................................................................ 33
User Interface ............................................................................................................................... 34
Form Design .................................................................................................................................. 35
Lesson 3................................................................................................................................................. 43
Building Rules .................................................................................................................................... 45
Variables........................................................................................................................................ 46
Variable Categories ....................................................................................................................... 47
Model Rules .................................................................................................................................. 51
Running your Project .................................................................................................................... 60
Layout Mode ................................................................................................................................. 63
Lesson 4................................................................................................................................................. 65
Improving Your Project ..................................................................................................................... 67
File Name and Relative Path Rules ............................................................................................... 67
Lesson 5................................................................................................................................................. 75
Static Replacement Files ................................................................................................................... 77
Lesson 6................................................................................................................................................. 83
Tables ................................................................................................................................................ 85
Lesson 7................................................................................................................................................. 91
Form Navigation................................................................................................................................ 93

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Lesson 8................................................................................................................................................. 97
Enhancing Your Forms ...................................................................................................................... 99
Dynamic Replacement Files ............................................................................................................ 102
Lesson 9............................................................................................................................................... 108
Driving Custom Properties .............................................................................................................. 109
Lesson 10............................................................................................................................................. 115
Documents ...................................................................................................................................... 117
Lesson 11............................................................................................................................................. 125
Drawings ......................................................................................................................................... 127
Capturing Drawing Detail ............................................................................................................ 127
Building Rules for the Drawing ................................................................................................... 137
Appendix ............................................................................................................................................. 144
Preparing Your Models for Automation ..................................................................................... 144
Glossary ............................................................................................................................................... 147

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Imagine you design Wooden Doors

If you worked for a Company that designed wooden doors, where each one you designed was
different, then you could use DriveWorks Solo to automate each design.

This training will show you how.

First let’s look at the design.

As you can imagine, the hole that a builder leaves in a wall could be any size (within reason) and
because this is a wooden door, each piece of wood needs to be designed and a drawing produced.

We will need to create a set of forms for someone to fill in, which will guide them through the
selections we make available to them.

That way we know that whatever they enter can be manufactured.

Also, it would be great to be able to produce a General Arrangement drawing automatically that
shows the exact requirements.

There will be rules that take the opening dimensions and calculate the sizes of each component.

We also need the ability to have a round or rectangular window in the door, which could also be a
custom size.

The steps required to do this in DriveWorks Solo are as follows:

Basic Setup

Create a project to store all the data.

Capture Models and Drawings

Decide which Models and Drawings will be driven, and what is driven in each case.

Form Creation

Create forms for our users to enter data to specify a new door and frame.

Rules

Add rules to drive the models and drawings from the inputs on the form.

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DriveWorks Solo
Design Automation
for SOLIDWORKS
Lesson 1
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Basic Setup
At this point you should have DriveWorks Solo installed and licensed.

If not, please visit https://hub.driveworks.co.uk/. Log into your account to download DriveWorks
Solo.

Opening DriveWorks Solo

DriveWorks Solo resides on its own tab in the SOLIDWORKS Task Pane. To open DriveWorks Solo,
enable and expand the Task Pane, and then click on the Solo Tab.

Alternatively, select DriveWorks Solo from the Tools Menu in SOLIDWORKS, which will activate the
tab on the task pane for you.

Now we need to create a project to store our automation information.

Concept: Opening DriveWorks Solo

DriveWorks Solo stores the information that you enter in a Project. Each Project can drive any
number of models, or combination of models from a set of Forms. Each different product that you
wish to automate would normally have its own Project, unless the data entered to design each one
is similar or the same.

The project file has a .driveprojx extension, and also uses similarly named accompanying files.

Tip:

Ensure the DriveWorks Solo add-in is turned on in SOLIDWORKS. Open the add-in list found in Tools -
> Add-ins and check DriveWorks Solo. Checking the Start-up check box will mean DriveWorks Solo is
ready to use every time SOLIDWORKS is launched.

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Creating a Project
DriveWorks Solo incorporates a wizard for creating and opening projects. At this point, we are only
dealing with creating Projects.

Concept: Help links

DriveWorks Solo uses help links to guide you through the setup of your automation products. The
links will either be a way to perform an action, or a link to the Help File covering the relevant topic.
Either way, it’s a great idea to click on the links.

1. Click on the link Please open a project before continuing at the top of DriveWorks Solo to
launch the Open/Create Project wizard.

2. Select Create a new project from the options and click Next.

There are now three options for creating a new Project:

• Empty Project

This will create an empty Project that you can add your own models to.

• Import from DriveWorksXpress

If you already have models captured in DriveWorksXpress, you can import them into
DriveWorks Solo.

• Using a Template

DriveWorks Solo ships with built in templates. These are great for getting to know
DriveWorks Solo and investigating a completed Project. More templates can be downloaded
from the Sample Projects section of the DriveWorks Solo website.

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For now, we are going to create an Empty Project

3. Select Empty Project from the list, and click Next.

4. Click Browse to select a location for your Project.

5. Browse to the location that you wish to store your Project.

It doesn’t matter where you store the Project, although for this training, browse for the same
location as the Door and Frame models that were shipped as part of this training. If you do not have
these files, you can download them from the DriveWorks Community https://hub.driveworks.co.uk/

Concept: Input Validation

DriveWorks Solo applies validation in all important areas. If you see the warning icon next to a text
box, hover over it to see a validation and hint tooltip. You will also be prevented from proceeding
until the validation criteria are met.

DriveWorks Solo will automatically use the folder name for the name of the Project. Type a new
name if required.

6. Click Finish to create the DriveWorks Solo Project in the chosen location.

You will now have a Project open, and a link at the top of the DriveWorks Solo Task Pane indicating
the next step.

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Capturing your Models

To capture a model inside DriveWorks Solo, a SOLIDWORKS Model needs to be open. If you do not
have any models open in SOLIDWORKS, the helper link will ask you to:

Open a model to capture it

7. Click the link, and browse for the SOLIDWORKS Part or Assembly that you wish to
automate. For this training, browse for the SOLIDWORKS assembly Wooden Door and
Frame.SLDASM that was shipped with this training material. Rebuild and Save the
Assembly once opened to update the file to your version of SOLIDWORKS.

With the Wooden Door and Frame model now open, the link at the top of DriveWorks Solo will
change to:

Click here to capture the current model

8. Click the link to capture the current model.

Once captured, the Task Pane will show all of the options for capturing model information in the
Capture Explorer.

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Captured Assembly Structure

Concept: Capturing

Capturing is split into different sections that appear at the bottom of the DriveWorks Solo Task Pane.
Click on each section header to activate the required section.

Click and drag the bar to resize the section headers as you become more familiar with their use.

Another link will now appear at the top of DriveWorks Solo stating that No components are captured
in this assembly. If clicked, the Help File will open at the relevant page.

This step controls which of the models in the main assembly are controlled by DriveWorks Solo. It is
not always necessary to capture every component or sub assembly, often standard components like
fixings and other hardware don’t need to be captured.

9. With the Captured Assembly Structure Tab selected, check all of the models in the tree
except any of the hinge models and the lock in the Door Assembly. These files will not be
driven or controlled as part of this training, and therefore do not need to be captured.
Save your project.

Note:

If you check a part in a sub assembly, the sub assembly will automatically be checked as well.

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Capturing Individual Models

This section involves selecting each captured model in turn, and then capturing each parameter to
be controlled inside that model. The parameters that can be captured for each Part or Assembly are:

Dimensions and Features

Captured dimensions and features are given their own name in DriveWorks Solo, to make it easier to
build rules for them later on. Each feature can also have its advanced properties captured, the
advanced feature properties that can be captured vary depending on the feature type.

For instance, if you choose to drive a sheet metal feature, you will be able to capture properties such
as its K factor, or Bend Table.

Custom Properties

Select an existing custom property in your model to be able to control its value dynamically, or add a
new custom property into your model, that will be driven.

DriveWorks Solo has three special custom properties that, if used, will allow you to drive the Color,
Material or Texture from a rule.

Drawings

Browse for the Drawings that you want to generate with your new SOLIDWORKS models. You can
have more than one Drawing for each part or assembly. Once captured, each Drawing can then be
further controlled and will be generated every time the component they are attached to is
generated.

Instances

Select different instances inside an Assembly that you want to control.

Instances can be suppressed, unsuppressed, deleted or swapped out for either driven replacements
or static replacements based on rules.

Replacement Models

Rather than overload your master models with every permutation of model that you would ever
need, DriveWorks Solo allows you to browse for replacement models that will be swapped into the
assembly based on your rules.

File Formats

When DriveWorks Solo creates new variations of your SOLIDWORKS files, you can also choose to
export those files to other file formats (for example eDrawings, STL and PNG)

Run

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From Run Mode you can specify complete Projects from the Local and Recent folder. Or install and
run a sample project from the samples folder. When a running Project is finished, a dialog will
appear that lets you choose the outputs you want to generate.

Concept: Captured Models

The Captured Models section shows all the models which have been captured in the currently open
project. Double click a model in the tree to open it in SOLIDWORKS.

10. Activate the Captured Models section by clicking on its heading within the Capture
Explorer.

Capturing Component – Wall

11. Expand the tree and double click on the Wall in the DriveWorks Solo Task Pane to open it
in SOLIDWORKS.

This will also automatically change the Task Pane to the Dimensions and Features Section.

This section controls which of the dimensions and features are controlled by DriveWorks for each
component you selected in the previous section. You do not need to capture dimensions and
features for every component.

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Concept: SOLIDWORKS Naming Convention

SOLIDWORKS has its own name for each dimension or feature. This next step ensures that each
captured item has a name that means something to you.

Selecting dimensions and/or features in the model or SOLIDWORKS feature tree adds the
SOLIDWORKS Address to the Address text box in the DriveWorks Task Pane.

Concept: Design Intent

At this point, you need to understand the design intent that we have applied to the models. We
have mostly used planes in the models and then attached the sketch geometry to the planes.
Changing the plane offsets therefore changes the size of the model.

At the end of this training there is a section on modeling for automation, that you can apply to your
models.

For now, we have listed below where each dimension or feature can be found in the model.

For the Wall, we are going to capture the opening size. This is driven by 2 planes called SOW and
SOH. (These stand for Structural Opening Width and Structural Opening Height)

To allow you to select the dimensions for these, you need to double click each plane in turn and then
select the dimension that appears.

Tip:

If you double click the TEXT of the plane, SOLIDWORKS will prompt you to change its name. Don’t
do this. Instead, double click on the icon for the plane. If you do this, you will see the dimension
of the plane appear in the model window.

12. Double click on the icon for the Plane SOW and click on the dimension that appears. The
SOLIDWORKS name for this dimension will appear in the DriveWorks Solo Task Pane.

The icon in the Solo tab will indicate what you’ve selected. In this instance, make sure that you have
selected the dimension and not the plane!

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Tip:

If you are having problems selecting the dimension, you may have Instant3D switched on. This will
prevent you from selecting dimensions for capture in the model window. If this is the case, a link
will appear in the DriveWorks Solo Task Pane. Turn Instant3D off to continue.

13. In the Name text box, enter Structural Opening Width and then click Add.

14. Follow the same principal for the SOH plane, and for its dimension. Give it the name
Structural Opening Height.

15. Click Add again.

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Both dimensions can then be seen in the tree view.

We have now finished capturing the parameters of the Wall.

Now let’s capture the Frame. This is made of 2 parts; both have a dimension that needs to be
captured.

16. Activate the Captured Models section by clicking on its heading within the Capture
Explorer.

17. Double Click the model Top Door Jamb in the Task Pane Tree.

Note:

You will need to expand the Frame Assembly to access the two captured parts, Door Jamb and Top
Door Jamb.

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Capturing Component – Top Door Jamb

This will open the model Top Door Jamb in SOLIDWORKS and, because this is a part, it will select the
Dimensions and Features section.

The dimension that you need to drive the length of this component is in the plane called Top.

1. Double Click on the Top plane in the SOLIDWORKS Feature Tree to show the dimension in
the model window.

2. Select the dimension in the model window and enter the name Length.

3. Click Add to capture the dimension.

There are no features to control in this part, however we do want to be able to control some custom
properties.

4. Select the Custom Properties Section Header.

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To capture existing custom properties, check them in the list. You will then be able to create a rule
for each captured custom property.

5. Check the custom property Date.

6. Check the custom property Description.

To add a new custom property to the model, and capture it at the same time, enter the name in the
text box and click Create.

7. Enter DWColor in the text box and click Create.

Concept: Custom Property Special Names

DriveWorks Solo has special names for some custom properties. These allow you to control the
color, material and texture of your models and are DWColor, DWMaterial and DWTexture

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respectively. These are not case sensitive, and DWColour can be used instead of DWColor based on
your spelling preference.

The second frame part is called Door Jamb.

8. Activate the Captured Models section by clicking on its heading within the Capture
Explorer.

9. Double Click the model Door Jamb in the Task Pane’s Captured Models Tree.

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Capturing Component – Door Jamb

This will open the model Door Jamb in SOLIDWORKS and, because this is a part, it will automatically
select the Dimensions and Features section.

1. Double click on the Plane called Top and select the dimension. Call this Length. Click Add.

Even though you have already used the name Length in a different component, you can use the
same name in as many different components as you wish.

2. Create a new custom property named DWColor for this model.

The next component is the wooden door itself. As well as dimensions, the Door also has features
that will need controlling.

Let's capture the dimensions first.

3. Activate the Captured Models section by clicking on its heading within the Capture
Explorer.

4. Double Click the model Wooden Door in the Task Pane Tree to open it in SOLIDWORKS.

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Capturing Component – Wooden Door

1. Capture the following dimensions. You will find some of the planes in a feature folder
called Reference Planes

The dimension in the Plane Bottom – Call the dimension Height.

The dimension in the Plane Right – Call the dimension Width.

2. Double click on the feature called Square Cutout. Capture the two dimensions that define
the sketch as Window Height and Window Width.

The next step is to capture the window cutout, so that we can choose to have a window or not.

3. Select the feature Square Cutout in the SOLIDWORKS feature tree.

Notice that the name of the feature is automatically added to the Name text box. This happens
because DriveWorks Solo recognizes when the name of a feature has been changed from the default
name given by SOLIDWORKS.

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4. Click Add to capture the feature.

Note:

This also happens with dimensions. If you have already named a dimension in SOLIDWORKS,
DriveWorks Solo will pick up on that name and enter it into the Name field automatically.

You should now have the parameters captured in line with the picture below.

The final item to capture on the door is to add a driven custom property called DWMaterial. This
will allow us to drive the material of the door based on rules.

5. Select the Custom Properties Section Header.

6. Enter DWMaterial in the text box and click Create.

You may have noticed the filter box underneath the header on the Task Pane. This allows you to
filter the list. It is particularly helpful when you have a lot of custom properties, and the list needs
filtering for ease of selection.

The last model to capture at this stage of the training is the Rectangular Window.

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7. Activate the Captured Models section by clicking on its heading within the Capture
Explorer.

8. Double Click the model Rectangular Window in the Task Pane Tree to open it in
SOLIDWORKS.

Capturing Component – Rectangular Window

Note:

To open the Rectangular Window, you may need to expand the Door Assembly.

9. Double Click on the feature Boss-Extrude1 in the SOLIDWORKS feature manager. Capture
the two dimensions for the overall size of the window (they are both 590), calling them
Width and Height.

The final task is to associate a Drawing with the top level assembly.

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10. Click on the Captured Models Section Header to show all of the captured models within
this Project.

11. Double Click the model Wooden Door and Frame in the Task Pane Tree.

This will open the model Wooden Door and Frame in SOLIDWORKS and automatically select
the Dimensions and Features section.

12. Click on the Drawings Section Header.

Concept: Associated Drawings

For each new part or assembly that you create from your masters in DriveWorks Solo, you can have
one or more Drawings associated with it. These will also then be created based on master drawings.
The Drawings section of DriveWorks Solo allows you to reference which drawings will be generated
for each part or assembly.

13. Browse for the drawing Wooden Door and Frame.SLDDRW in your training files folder.

All of the models we need for now have been captured. The next step is to set up a user form to
allow specification information to be entered.

To save your DriveWorks Solo data click on the save button on the DriveWorks Solo Command Bar.
This will save your Project data, but not the SOLIDWORKS files. Click the SOLIDWORKS save button
to save your models.

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DriveWorks Solo
Design Automation
for SOLIDWORKS

Lesson 2
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Project Designer
DriveWorks Solo has an inbuilt Project Designer that allows you to create your forms, create tables
of data, build rules for your models, and configure your quotation.

The Project Designer is split into 3 sections in the Task Explorer:

• Stage 1: User Interface

Set up the navigation through your forms, and design each form using the inbuilt
form controls

• Stage 2: Data and Rules

Create tables, and build variable rules that will be re-used within your Project

• Stage 3: Output Rules

Create and manage the rules for driving your models and drawings, as well as
the rules for creating dynamic documents

The Project Designer also has a command bar that will show in-context tools relevant to the section
you are working on.

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User Interface
The user interface section is split into two elements:

1. Form Navigation

Here you will set up the dynamic navigation through the forms of your Project. Rules can be
used to set the navigation based on other inputs, allowing you to guide a user through
relevant forms.

2. Form Design

Use the inbuilt controls to create your form. Form controls have dynamic properties that
allow you to build rules that will dictate their behaviour.

Concept: Form Design

DriveWorks Solo can use multiple forms to specify new variations of your products. These forms are
linked together using Form Navigation.

Form Navigation

Whenever you create a new Project, DriveWorks Solo creates the first form for you, and creates the
navigation from start to finish.

Concept: Form Navigation

Navigation requires a Start and a Finish. This ensures that you always have a starting point when
you start using the forms to create your new models. The finish point lets DriveWorks Solo know
when to show the finish button so that you can finalize your design and documents.

The default navigation, with a single form, looks like this:

The command bar has buttons specific to form navigation, including alignment tools to help tidy up
your navigation, and buttons for adding, deleting and renaming forms and decisions.

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Concept: Navigation Decision

A Decision is a two way splitter that allows you to show one of two forms based on a single rule.

At this point in the training, we are going to just use the default form with no decisions. These will
be covered later in the training.

1. Open the Project Designer by clicking on the toolbar at the top of DriveWorks Solo.

Form Design

2. Activate the Form Design by selecting the Form Design task in the Task Explorer.

The form designer will default to showing the first form. In this case, there is only one.

Tip:

You can also right-click on the form icon in the Form Navigation stage and select Go To Form
Designer.

The form is empty. You can now start adding Form Controls.

Concept: Command Bar Overflow

If you shrink the Project Designer’s width, buttons on the Command Bar will automatically be moved
to the overflow menu.

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Form Controls
Concept: Form Controls

Adding inputs to each form is done by clicking on the appropriate button on the Command Bar
above the form designer. A text box then appears asking for a name. You cannot use the same
name twice, and it is good practice to use meaningful names. Names cannot have spaces in them.

Numeric Text Box

1. Click on the Numeric Text Box button on the Command Bar. A text box will appear asking
for a name for the Numeric Text Box. Call it OpeningHeight.

2. Click the OK button to create the control.

The caption for the text box will be as you typed it, with no spaces. This can be changed by updating
the value for Caption in the properties pane. However, if your name has capitalized words, such as
OpeningHeight, then DriveWorks Solo will recognize this and add in spaces in the caption.

Concept: Control Properties

If you select the control on the form, the properties pane on the right will show you all of the
properties that you can set for the type of control that you have selected. Some properties are
static, which means that you set them and they stay that way until you edit them again, and some
are dynamic, which means you can build rules for their value.

Each Form control has Static and Dynamic Properties.

By default, Static Properties include font, color and size.

Dynamic Properties can include properties like the visibility or whether a control is enabled or
disabled. Different controls have different properties. For example, controls such as labels have text
properties whereas controls such as combo boxes, lists and option groups have list properties.

Static properties are shown with a grey icon, while dynamic properties have a green icon.

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Set the following values shown in the image above for the 2 Properties Maximum and Minimum:

Maximum = 2100
Minimum = 1700

Spin Button

3. Create a spin button called OpeningWidth.

Concept: Alignment Guides

Alignment Guides control alignment snapping in the Form Designer while dragging a control (or
group of controls). To temporarily disable the snapping, hold down the Ctrl key whilst dragging the
control.

A spin button requires a minimum and maximum value, as well as an increment.

These are entered in the Property Pane on the right-hand side of the Form Designer. Make sure you
have the correct control selected in the Form Designer when you are changing these values.

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Set the following values shown in the image above for the three Properties Maximum, Minimum and
Increment:

Increment = 50
Maximum = 1500
Minimum = 900

Concept: Static and Dynamic Values

You may have noticed that when you type in the values for Minimum, Maximum and Increment, that
a button appears to the right of the box. Clicking this button will open the Rules Builder, which
means that rather than being static, you could have dynamic values for your properties. For
instance, the minimum width may change if the door goes above a certain height.

Leave them as static values for now.

I’m guessing that curiosity has got the better of you, and you have opened the Rules Builder. Click
Cancel, we will get to the Rules Builder shortly.

Combo Box

4. Create a Combo Box called Window.

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Concept: Combo Box

A Combo Box is a drop down list where any value can be selected. The list in the drop down can be
static or dynamic.

In order to populate the list of items the Combo Box offers, we need to enter a value for its Items in
the Property Grid.

Concept: Lists

Lists in DriveWorks Solo are usually represented by a single string, each item within the list is
required to be separated by a pipe bar (|). So, for example, if you want a list with Monday, Tuesday
and Wednesday as static values, you would need to enter "Monday|Tuesday|Wednesday".

To create the List needed to populate the Combo box, we are going to use the Rules Builder.

5. Click in the Items property for the Combo Box. A button will appear to the right of the
property value.

6. Click the button to launch the Rules Builder.

Tip:

You need to click in the Items property for the button to appear.

Rules Builder
The Rules Builder is split into numerous sections, with its own Command Bar, a Rule Editor, Help and
Diagnostics and a browser to find your Project Variables and Form Values.

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The rule is entered into the Rule Editor, using a combination of typing, the helper functions on the
command bar, and by double clicking on Form and Variable entries.

In this case, because we want static values in the Combo Box, we are just going to type in the text
"None|Rectangular".

7. Click in the Rule Editor and Type "None|Rectangular".

Note:

Since this is static text, make sure that you include the quote marks.

8. Click OK on the Rules Builder. The rule will appear in the Items property in the Property
List.

Add More Controls

For now, we need to add two more Form Controls that will allow the size of the rectangular window
to be specified.

9. Create a Numeric Text Box control called WindowWidth.

10. Set the properties for Minimum and Maximum to be 200 and 600 respectively.

11. Create a Numeric Text Box control called WindowHeight.

12. Set the properties for Minimum and Maximum to be 200 and 600 respectively.

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Your Form is now ready, so we can move on to the Model Rules that will link your Form Values to
the information that you have captured in your models.

You should now have a form that looks a bit like this:

Note:

One way to control the position of each Form Control is to select them on the Form Canvas and drag
the Form Control to the required position.

Concept: Group Controls

Controls can be grouped together to reposition. Select a control then hold down Shift or Ctrl while
selecting other controls. Right click and select Group Controls to group them together. To ungroup,
select any control within the group, right click and select Ungroup Controls.

Have a go at changing some of the static properties for each control. Also experiment with the align
tools at the top of the Form Designer.

Clicking the Test Mode button at the top of the Form Designer also allows you to see what the form
will look like when it is being used to configure a new product.

Clicking Test again returns you to Design Mode.

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Note:

Any Values you enter into your Form Controls in Test Mode will become the default values for those
controls.

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DriveWorks Solo
Design Automation
for SOLIDWORKS
Lesson 3
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Building Rules
Let’s look at the models. In the following picture, all sizes have been exaggerated.

From this picture, it is easy to see that to calculate the width of the door you need to take into
account the Opening Width, Wall and Frame Gap, Frame Thickness and the gap between the door
and the frame.

So, the rule would be in this form:

DoorWidth = OpeningWidth - 2 * (WallandFrameGap + FrameThickness + DoorandFrameGap)

Our Form already has an input for the Opening Width, and in this case, the other values will be
static.

It would be very straight forward, knowing the static values, to just type them in, so that the rule
would be:

DoorWidth = OpeningWidth - 2 * (5 + 40 + 5)

Or even:

DoorWidth = OpeningWidth - 100

And there would be nothing wrong with that, except that if we ever wanted to change any of the
gaps, or even make them dynamic in the future, we would have more work to do, and our project
wouldn't be as flexible.

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It also makes it easier to track and validate your rules, as they will have a name that can be
understood easily.

It's therefore better to enter all of these static values as variables, and then use them in a rule.

Variables
DriveWorks can store values for use in your rules.

Let’s add the gaps around the door and frame as Variables.

1. Select the Define Variables task in the Task explorer.

2. Click Add Variable to create a new Variable.

Note:

As with creating new Forms, a text box will appear asking for a name for your new Variable. Again,
validation is used to ensure your name is valid.

3. Enter WallandFrameGap for the new Variable name and hit Enter.

You will see the new Variable added to the list:

Note:

You can change the name of a Variable at any time by slowly double clicking on the name in the list.
You will be asked to confirm the action because when the name is changed, DriveWorks Solo will
need to search through every rule in your project to see where that variable has been used, and
update those rules where it is found.

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4. Enter a value for the Variable by double clicking in the Rule column.

5. Type in a value for your variable of 5 and hit Enter.

Note:

You can also enter the value in the Rules Builder by either double clicking in the Value column, using
the Build button on the Command Bar, or by selecting the Variable and using the keyboard shortcut
Ctrl + B.

6. Add another Variable, name it DoorGap, and give it a value of 5.

7. Add another Variable, name it FrameThickness, and give it a value of 40.

Variable Categories
Concept: Variable Categories

Variables can be sorted into categories. This can be used to group similar Variables, making them
easier to find after many have been added to a Project.

8. Click the Add Category button on the Command Bar.

9. Enter the name Sizes and click OK.

Tip:

You can also hit the Enter Key to accept your name, as long as your name is valid.

This adds your category to the tree.

To add new Variables to this Category, select the Category in the tree before clicking New Variable.

To add existing Variables to a Category, drag them onto the Category item in the tree.

10. Drag all 3 Variables that you have just created into the new Sizes Category

We can now set Variables for the Frame width and height, as well as the Door width and height.

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11. With the sizes category selected, click Add Variable to create a new Variable in the new
Variable category.

12. Give the Variable the name FrameWidth and hit Enter.

13. With the FrameWidth row selected, click Build on the Command Bar to launch the Rules
Builder.

Have a click around inside the Rules Builder. You will see your Form Controls, as well as your new
Variables in the Browser on the right. We will be adding the rule for the FrameWidth Variable:

OpeningWidth - (2 * WallandFrameGap)

Although you do not need to type this in.

Concept: Control and Variable Double Clicking

Double Clicking on an item in the Controls and Variables Browser will add its name to the Rule
Editor.

14. From the Controls tab on the right, double click on the name OpeningWidth. This will add
the text OpeningWidthReturn to the Rule Editor.

Note:

DriveWorks Solo adds the word Return as a suffix for Form Controls. The ‘return’ is referring to the
value entered into the control.

15. Then type a minus sign, followed by an open bracket - (

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Note:

Calculations performed by DriveWorks Solo respect the mathematical order of operations. However,
in this case brackets are simply being used to make the rules easy to read which can be useful when
editing existing rules.

16. Then type 2 * and switch the Tab on the right to Variables and double click on the Variable
WallandFrameGap followed by a closed bracket )

Note:

DriveWorks Solo adds the word DWVariable as a prefix to identify Variables.

17. You should now have a rule that looks like this:

18. Click OK to accept the rule.

19. Create another Variable called DoorWidth using the rule:

DWVariableFrameWidth –
(2 * (DWVariableFrameThickness +DWVariableDoorGap))

20. Click OK on the Rules Builder to accept the rule.

Tip:

It is much easier to double click on the Variable in the Variable Browser on the right, rather than
typing it in manually. If you find you have a lot of Variables, use the filter box to limit the Variables
displayed.

21. Create another Variable called FrameHeight and use the rule:

OpeningHeightReturn - DWVariableWallandFrameGap

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Note:

You can change the appearance of the Rule Editor by clicking on the Settings button on the
Command Bar.

22. Create another Variable called DoorHeight using the rule:

DWVariableFrameHeight - DWVariableFrameThickness - (2 * DWVariableDoorGap )

Concept: Rules Builder Diagnostics

The Rules Builder has diagnostic tools built into it, to help you create accurate rules quickly. At the
bottom of the Rules Builder you will see a Diagnostics area. On this there are 4 tabs:

Values - All the individual elements that make up the rule are displayed here, to help you check your
rule. Also included here is the current result of the rule.

Steps - Here, each rule is broken down into sub rules, so that you can quickly see the cause, if you
are not getting the result that you expect.

Drill Down - The drill down tab provides the information used in the values and steps to be analyzed,
you can expand the rule at each stage to get to the result.

Comment - You can enter a comment for each rule.

You should now see the following Variables in your list.

Note:

Depending on the default Form Control values you entered when testing your Form, you may have
different results for your Variables.

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Model Rules
We are now ready to build some model rules, and then create some new SOLIDWORKS files based
on the information we enter in the form.

The first step though is to tell your DriveWorks Solo Project which models to control.

Concept: Adding Captured Models to the Project Designer

Captured Models are not automatically added to the Project Designer, as you can choose to drive No
Models, One Top Level Model or More than One Top Level Model.

Therefore, you need to tell your Project which models to use.

23. Select the Model Rules task in the Task explorer.

Note:

As you haven’t added any models to your Project yet, the Add Component dialog will automatically
appear. You can also select Add from the Command Bar to launch the Add Component dialog.

24. Check the box for the assembly Wooden Door and Frame and click OK.

You will now see the Wooden Door and Frame added into the Component Tree.

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Note:

You only need to add the top level assembly. All of the captured sub-assemblies and parts will be
added to the tree automatically. It is possible to choose the specific models you want to add by
checking, and unchecking, the relevant check boxes.

25. Right-click on the Wooden Door and Frame in the tree and click Select Children.

This will show all of the rules for all of the added components.

Note:

Selecting a component in the Model Rules tree will provide information about the captured master
model it is associated with at the bottom of the Project Designer window, under Component Details.

You will notice that some rules have already been filled in. Specifically, the File Name and Relative
Path rules.

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Concept: File Name and Relative Path

File Name is the rule that will determine the name of the file that will be created when you run your
project.

Relative Path is the rule for the location of the new file relative to a folder called Results which will
be created inside your Project folder.

The default given for these is the name of the Project, followed by an incremental number (shown as
9999 during the design of your Project for testing purposes).

For the File Name, the result of this rule will be appended to the original file name of each master
model.

For example, for the top-level assembly Wooden Door and Frame, when the Project is run for the
first time, a new assembly file will be generated and saved with the name Wooden Door and Frame
DriveWorksSoloTraining 1.SLDASM in a folder named DriveWorksSoloTraining 1 in the Results
folder.

We will be changing these rules later in the training, but for now we will leave them as they are.

Each Model has a rule for Configuration. Only create a rule for these if you wish to change the
configuration you wish to use in your model.

Let's create rules for the dimensions first.

Rather than scroll up and down looking for the dimension rules, you can type a filter in the filter box
at the top of the Rules List.

26. Type dim in the filter box to only show rules with dim in any of its values.

27. Select each one in turn, click the Build button on the Command Bar and, using the table
below, create a rule for each dimension.

Since we have been to the effort of creating Variables for most of these, or because we are using a
direct link from some Form Controls, the model rules are very straight forward. We will add more
complicated rules later in this training, but for now set the following rules.

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Tip:

If you multi-select rules in the Model Rules List (by holding down Shift or Ctrl while selecting with
the mouse) and then click Build, you can build all the selected rules at once. If one of these rules
already has a rule, that rule will be displayed in the Rule Editor.

Name Component Rule

Height Rectangular Window (Part) WindowHeightReturn - 60
Height Wooden Door (Part) DWVariableDoorHeight
DWVariableFrameWidth –
Length Top Door Jamb (Part)
2*DWVariableFrameThickness
Length Door Jamb (Part) DWVariableFrameHeight
Structural Opening Height Wall (Part) OpeningHeightReturn
Structural Opening Width Wall (Part) OpeningWidthReturn
Width Rectangular Window (Part) WindowWidthReturn - 60
Width Wooden Door (Part) DWVariableDoorWidth
Window Height Wooden Door (Part) WindowHeightReturn
Window Width Wooden Door (Part) WindowWidthReturn

Variables do not require pre-creating in Define Variables to be used elsewhere. The Rules Builder can
be used to create variables quickly using the Extract Variable feature.

28. In the Model Rules double click the Length for the Top Door Jamb Part to open the Rules
Builder.

29. Highlight the rule, right click and select Extract Variable. Name the new variable
TopDoorJambLength.

If you select the Replace in all rules check box an additional dialog will be displayed to allow you to
specify which occurrences of the rule you wish to change throughout the project.

You will see that the old rule has now been replaced by the new DriveWorks Variable we created.
The new Variable can be found in the Define Variables section of the Task Explorer. Make sure you
finish building the Length rule for the Top Door Jamb by clicking OK.

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30. Click on the Name column header to sort the name in ascending order.

Your dimension rules should now look like this:

Note:

Your Value column may be different as they are calculated using default Form Control values setup
in Test Mode.

Again, don't worry if the Values differ from your own as these will depend on the values entered on
your Form in Test Mode.

31. Change the filter box text to be feat to show the rule for the feature that we captured.

We want to Suppress or Unsuppress this feature based on the Combo Box we added earlier.

32. Click on the Square Cutout feature.

33. Click Build on the Command Bar to launch the Rules Builder.

34. You will see a new Help Tab on the Help and Diagnostic section at the bottom of the Rules
Builder.

Tip:

Click on this tab to see Help specifically related to the type of rule that you are building.

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35. The rule will be using logic, known as an IF function. The Rules Builder has built in
Function Wizards to assist you when building functions.

36. Click on the arrow at the bottom of the Functions button on the Rules Builder Command
Bar.

37. Click on the IF entry to activate the Function Wizard at the bottom of the Rules Builder.

For an IF function, three text boxes allow you to enter the three arguments.

These arguments are:

IF This is the condition that will be evaluated

Then If the condition is evaluated to be TRUE, use this value

Otherwise If the condition is evaluated to be FALSE, use this value

We are going to enter the following

IF WindowReturn = "Rectangular"

Then "Unsuppress"

Otherwise "Suppress"

This means that if the Combo Box value is set to Rectangular, then the feature will be Unsuppressed
(it may already be unsuppressed, in which case no action will be taken), and if it isn't set to
Rectangular, then it will be Suppressed.

Tip:

If any of the three text boxes on the function wizard have focus, then double clicking on an item in
the Form and Variable Browser will add that item to the focused text box.

38. Click in the Condition text box on the Function Wizard.

39. Browse to the Controls on the right, and double click the Window Control Name.

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40. Then type ="Rectangular"

41. Click in the Value If Condition Is True text box on the function wizard and type
"Unsuppress".

42. Click in the Value If Condition Is False text box on the function wizard and type
"Suppress".

43. Click Finish to add the function to the Rule Editor.

44. Click OK to apply the rule.

Concept: Quick Text

If you have text that is likely to be entered in to the Rule Editor numerous times, you can store it as
quick text. Click the Quick Text button on the Rules Builder Command Bar, and type in your
frequently used text, hitting return between each item.

Once you close the Quick text Dialog, clicking on the arrow will display your Quick Text. Click on the
text to add it to the Rule Editor.

The last rule we are going to build at this stage of the training is to suppress the Rectangular Window
model, if the Form value is set to be "None".

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45. Click the Refresh button on the Command Bar to clear the currently selected components
and clear the rules List. You will also need to clear the filter that was previously applied to
show all the parameters for this component.

46. Expand the Component tree and check the item Rectangular Window. The rules list will
now only show the rules for the selected component.

We are going to change the File Name rule to Suppress the rectangular window Component when
the Form Control’s value is "None".

47. Select the Rectangular Window File Name row.

48. Click Build to launch the Rules Builder.

49. Clear the current rule by clicking on the Clear button on the Command Bar.

50. Use the IF Function wizard again by clicking on the arrow under the Functions button, and
selecting IF.

51. Enter the following values in the three text boxes of the Function Wizard.

IF WindowReturn = "Rectangular"

Then DWSpecification

Otherwise "Suppress"

Note:-

DWSpecification is a special variable used by DriveWorks Solo that is made up of the Project Name
followed by a sequential number that is incremented each time you start a new specification.

It can either by typed in manually, or added automatically by clicking on the arrow on the Quick Text
button, and selecting:

Special Variables>Specification Name

Note also that DWSpecification is a variable and therefore does not need quotes around it whereas
"Suppress" is static text, and therefore does need quotations.

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52. Click Finish to add the result to the Rule Editor and Click OK to apply the Rule.

The meaning of this rule, when applied to this file name, is that if the Window Form Control is set to
"Rectangular", then a new file will be created based on the master, with the Specification Name as a
suffix, otherwise the master model will simply be suppressed in the generated assembly.

Note:

Now you have your rules, you can sort and filter in several different ways.

Checking or Unchecking models in the Component Tree adds and removes them from the list.

Type in either the filter box above the Component Tree, or above the Model List to filter each one in
turn.

Click on any column header to sort by that column. Repeated clicks will toggle between sorting
ascending, descending and unsorted.

There are a few more rules we could build now for Captured Custom Properties, however we will do
this later in this training.

You should now be ready to create some new models based on your Form and Rules.

53. Close the Project Designer, and click Save on the DriveWorks Solo Command Bar at the
top of the SOLIDWORKS Task pane tab.

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Running your Project

You now have everything set up to run your Project and create new models.

1. Close any open models in SOLIDWORKS.

2. Click the Run Button in DriveWorks Solo.

Your Form will appear in the Task Pane Tab, and the buttons on the Command Bar will change to be
appropriate for running a Specification.

Note:

In addition to running a Project by filling out Forms manually, it is also possible to run a Project From
File. This is accessed by clicking the drop-down arrow next to the run icon.

Concept: Preview Button

When filling out your Forms in DriveWorks Solo, you can preview your models in SOLIDWORKS at
any time.

If you have previewed your models at least once, then you will also be able to preview any Drawings
that you captured for the top-level assembly.

You can also preview any documents you have captured. At this stage of the training, we have not
captured any documents.

3. Change the values on the form.

4. Click the Preview button on the DriveWorks Solo Command Bar to see your models being
created based on the inputs and the rules that you created.

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A copy of the top level assembly will now open in SOLIDWORKS, and all of the files will have been
given temporary file names.

Change the values on your Form, and click Preview again to see the updated model.

Note:

Once the models have been opened initially, the preview will work on the opened file.

Auto Preview
By clicking the down arrow next to Preview you can select Auto Preview. This will regenerate the
model each time a value is changed on the Form.

5. Click on the Generate Drawings button to see a preview of the Drawing that you captured
for the Wooden Door and Frame

Don't worry at this point if the scale of the drawing doesn't look great, or if there are misplaced
views or dimensions.

Controlling these will be covered later in the training.

6. When you have finished previewing your models and drawing, click Finish at the bottom
of your Form.

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A Finish Dialog will appear.

Uncheck the boxes for the results that you do not wish to create.

Click Finish to update all of the files with the correct names, and to save them into the correct folder.
At this point, DriveWorks Solo will create all of the drawings captured, and not just the ones
associated with the top level assembly.

Note:

The files that DriveWorks Solo creates during the previews have temporary file names and are
stored in a temporary folder. Even if you save them, they will be deleted after you click finish on
your Form, as they will already have been saved to the final location at that point.

Concept: Export form data

By leaving the Export Form data option checked, all the values manually entered on the Forms will
be saved in an XML file. This will be generated in the Project’s Results folder and can be used to re-
run a Project with existing values. You can go to the DriveWorks Solo Help File for more information
on how this works.

You may have noticed an issue with the Hinge Assembly when smaller doors are specified. We have
not captured the Hinge Assembly and therefore have not controlled the number or position of the
hinges. As an additional exercise, why not have a think about how this could be done and implement
it when you have some spare time!

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Layout Mode

Layout mode allows multiple DriveWorks Solo projects to be specified and automatically inserts each
model generated into an active top level assembly.

Layout Mode is not covered in this training manual. For further information see the DriveWorks Solo
Help File.

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DriveWorks Solo
Design Automation
for SOLIDWORKS

Lesson 4
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Improving Your Project

Once you have a project set up in DriveWorks Solo, you can keep adding more options.

For the remainder of the DriveWorks Solo training, we are going to update the Project and:

• Change the file naming and location Rules

• Use tabular data copied from Microsoft Excel

• Improve the Forms

• Add the option to have a Circular Window

• Drive model Colors, Materials and Textures

• Drive a SOLIDWORKS Drawing including driving the scale and view position

• Create a quotation document based on a template

File Name and Relative Path Rules

File Name: Where you build a rule for the name of the new model.

Concept: File Name Rule

DriveWorks appends the result of the rule for File Name onto the existing file name with a space in
between. So, if your original model is called Block and you have a rule that results in a value of 123,
then the new file will be called:

Block 123.

Relative Path: Where you build a rule for the location of the model.

Concept: Relative Path rule

The relative path is a file path that will be added onto the Results Folder, which is automatically
created inside your Project folder. So, if your Project Folder is set to be C:\DriveWorks\Projects and
your relative Path rule results in a value of Acme\123 then the new file will be placed in a folder
called:

C:\DriveWorks\Projects\Results\Acme\123\

Your Project Folder is simply the folder that your .driveprojx file is saved in.

Alternatively, you can build a rule to an absolute path (Local, Mapped Drive or UNC) and the new
model will be placed in that folder.

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Configuration: Where you build a rule for the configuration to use.

Concept: Configurations

DriveWorks does not create new configurations in parts and assemblies. Instead it creates new
copies of captured master files. However, DriveWorks can switch the used configuration based on
this rule, if the part or assembly has more than one configuration. If you do not want to select a
configuration to use based on a rule, then you can leave this rule blank.

First, we are going to add a Text Box to our Form so that an Order Number can be typed in, we will
then use that Order Number to name our files.

1. Open the Project Designer. If you are still running your Forms, either click Cancel or
Finish.

2. Go to the Form Design task in the Task Explorer.

3. Create a new Text Box on your Form called OrderNumber.

Since we are going to use this order number to name files, we need to make sure that whatever is
entered is valid for a file name. The first validation is to make sure that something is entered.

We do this by building a Form Warning using the Error Result dynamic property.

The Error Result rule will need to either calculate to be a text string, in which case that text string is
used as the Form Warning, or be calculated to be an empty text string which would mean that the
entry is valid.

4. Click in the Error Result property for the Order Number Text Box on the Property List.

5. Click on the button that appears which will launch the Rules Builder.

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6. Use the IF function Wizard to build the following rule:-

We can further enhance this by adding the function ISVALIDFILENAME, which will make sure that
valid characters are entered suitable for a file name.

Concept: Nested IF Functions

Nested IF functions are created by placing a completed IF function, with its 3 arguments, inside
either or both of the last 2 arguments of an existing IF function.

7. Update the rule to use a nested IF function as below.

8. Click the Function button on the Rules Builder Command Bar to find the ISVALIDFILENAME
function, or type it manually

The above rule has had carriage returns and spaces added to make it clearer to read. While this is
not necessary, it does help if you need to re-visit the rule at a later date.

9. Click OK to apply the rule.

Now we can link the file name of our models to this OrderNumber.

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10. Go to the Model Rules by clicking on Model Rules in the Task explorer

11. Right Click on the Wooden Door and Frame in the Component Tree and click Select
Children

12. Type File Name in the filter box at the top of the Rules List

13. Multi-select all the File Name rules (except for the rule for the Rectangular Window, we
have already changed that, so we will need to modify it separately).

Tip:

To multi select with exclusions, click the first rule, <shift>click (click with the mouse while holding
down the Shift key) the last rule and then <control>click the one to exclude.

14. Click Build.

You will see the existing rule DWSpecification in the Rule Editor.

For now, we are going to append the value typed in the OrderNumber field on our form, onto the
end of the original file name.

So, if we type QT123 into the OrderNumber field, the new version of this assembly will be called:

Wooden Door and Frame QT123

Note: - DriveWorks automatically adds the space between the original file name and the new suffix.

15. Click the Clear button on the Rules Builder Command Bar to clear the Rule Editor.

16. In the Form Browser on the right, double click on OrderNumber.

This creates the rule OrderNumberReturn.

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17. Click OK to save the rules. The Rules and Values will be updated automatically in the Rules
List. Unless you entered a value for OrderNumber when you created it, the value will
currently be blank.

18. Next, select the Rectangular Window File Name rule and click Build.

19. Double click on the word DWSpecification in the Rule Editor.

20. In the Form Browser on the right, double click on OrderNumber.

This will replace the selected text in the Rule Editor with the OrderNumberReturn

21. Click OK to apply the Rule

With the Order Number being used this way, and assuming an OrderNumber of QT543 is filled out in
the form, the following assembly structure would be produced.

There are a couple more things we could do at this stage with File Naming. We could decide not to
use the original file name in our new file name, or we could use a different rule so that the new file
name includes the parameters that drive it.

Let’s create a file name that does not use the original name.

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1. Right Click on the Wooden Door and Frame in the Component Tree and click Deselect
Children. Reselect ONLY the Wooden Door and Frame Assembly.

2. Select the Wooden Door and Frame file name rule in the list of rules, with nothing else
selected.

3. Click Build to launch the Rules Builder.

4. Before the text OrderNumberReturn, type in "*" &

5. Click OK to apply the rule.

Concept: String concatenation

You can link different rule elements together including Variables, Text Strings and Form Values, using
the ampersand character (&). Text Strings must be kept within double quotation marks.

The rule should now look like this:

"*" & OrderNumberReturn

Concept: Asterisk character

Having an asterisk (*) at the start of a file name rule tells DriveWorks Solo to exclude the original
name when it calculates the new file name.

Going back to the original example, we would now get the following results based on entering the
order number QT543:

Note:

The new name for the Wooden Door and Frame is QT543, not Wooden Door and Frame QT543.

We can now take this one stage further by building up a text string for the new name for the
component Top Door Jamb.

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6. Navigate to Define Variables and add a new Variable. Call it FrameColor.

7. Click the FrameColor variable and build a new rule. Type “Black” and click OK.

8. Navigate to Model Rules and select the Top Door Jamb from the list of models and select
its file name rule in the list of rules, with nothing else selected.

9. Click Build to launch the Rules Builder.

10. Click on Clear Rule and then build up a new rule using the Variables for FrameColor
together with FrameWidth and adding the word long on the end.

DWVariableFrameColor and DWVariableTopDoorJambLength are named values, and the word long
is plain text, the rule should look like this:-

DWVariableFrameColor & “ “ & DWVariableTopDoorJambLength & " long"

Notice the space in speech marks, the space after the first speech mark, and before the word long.

Now, based on a FrameColor of Black, OrderNumber of QT543 and an OpeningWidth of 1350

(which would calculate the variable DWVariableTopDoorJambLength to be 890), the new assembly
structure created by DriveWorks Solo would look as follows:

Note:

The driven name for the component Top Door Jamb Black 890 long.

Concept: Intelligent File Naming

DriveWorks Solo will use existing files if they exist, and create them if they don't. By using the length
in the file name, if DriveWorks Solo calculates that it has a requirement for the same file, it will not
be re-created, and the existing file will be used: improving generation time.

We can therefore change the Relative Path rule for the Top Door Jamb to place its files in a folder
called C:\MyModels\Standards

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11. Select only the rule for the Relative Path of the Top Door Jamb (you may need to remove
your existing filter). Filtering the Rule List or only checking the Top Door Jamb item in the
Component Tree may help you find this.

12. Click Build to open the Rules Builder.

13. Enter the new rule:

"Standards"

This rule will mean that all new Parts generated from the Top Door Jamb master model will be saved
in a folder called ‘Standards’ inside the Results folder.

14. Click OK to save the rule.

Note:

The folder structure inside a Relative Path rule is created using the \ separator. However, you
should not have a \ at the start or end of the Relative Path rule.

Placing a full file path in a component’s Relative Path rule, like "C:\MyModels\Standards", will
ignore the Relative Path convention and allow a file to be saved in any accessible location.

15. Close the Project Designer, click on the Save Button on the DriveWorks Solo Command Bar
and Specify more models by running the Project and filling out the Forms.

Note:

To see what impact the rules you have built have on generated files, take a look at the names and
locations of the files that your Project now generates.

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DriveWorks Solo
Design Automation
for SOLIDWORKS

Lesson 5
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Static Replacement Files

DriveWorks Solo has the ability to swap in replacement files for the files in your master assembly.

In order to do this, we need to tell DriveWorks Solo that replacement files exist.

1. With the Project Designer closed, make sure the lever handle part is open and is the active
document, either by opening it in SOLIDWORKS using the File>Open browser, or by double
clicking on it in the DriveWorks Solo Captured Models Section.

2. Once open, activate the Replacement Models section by clicking on its header in the
Capture Explorer.

In the Training files folder, there are files called Lever handle.SLDPRT and Ball handle.SLDPRT.

3. On the Replacement Models section, click the Browse button then browse for and add
these two parts.

This tells DriveWorks Solo that we may want to swap in the Ball Handle to replace the Lever Handle.

Now we need to tell DriveWorks Solo when to swap it in. For this we will need to add another Form
Control.

4. Click Save and Open the Project Designer, and go to the Form Design section by clicking on
the Form Design task in the Task Explorer.

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Option Groups

1. Add an Option Group to your form, giving it the name Handle.

Option groups behave in a similar way to Combo Boxes, in that they have a dynamic or static list of
options where you choose one from many when you fill out the form.

2. Build a rule for the Items property of your new Option Group

3. Type "Lever|Ball" in the Rule editor and click OK.

Picture Box

1. Add a Picture Box to your form. Call it HandlePicture. Picture Boxes have a File Name
property which use the Rules Builder to help create a file name.

Note:

The Picture File Name rule can either be a full path, or relative to your Project Folder.

2. Select the File Name property in the Property List, and click the button to launch the Rules
Builder.

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3. Click on the File button on the Rules Builder Command Bar.

4. Browse for the Ball Handle.jpg picture in the Content folder of the training files. If this
folder is relative to the Project Folder, then the path of the Project Folder will be removed.
This will help when you either move your Project, or distribute it to others.

This will now display the Ball Handle Picture at all times, unless we make it dynamic. We can do that
by editing the rule to use the selected Handle Option Group value.

5. Change the rule to:

"Content\" & HandleReturn & " Handle.jpg"

Notice that the word Ball has been replaced with a dynamic value, and since this is a combination of
static text and dynamic values, the ampersand (&) character is used along with quote marks.

6. Click OK on the Rules Builder.

Before testing the Picture Box Control, we need to change the Size Mode Property. The Size Mode of
a Picture box can be either:

Normal – The image is placed in the top left corner of the picture box and kept at its native size

Stretch Image – The image is placed in the top left corner of the picture box and is ‘stretched’ to fit
the size of the picture box

Center – The image is placed in the center of the picture box and kept at its native size

Zoom – The image is resized to fit the Size of the Picture box, but is not ‘stretched’, therefore
maintaining its aspect ratio.

7. Update the Size Model Property to be Zoom and resize your Picture Box to a suitable size

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Your Form should now look something like this.

Note:

You will need to reposition some of the Form Controls’ positions to produce a Form layout like the
one shown above. You can do this by dragging the existing Form Controls around the Form Canvas.

If you don't see the picture change based on your selection for handle, there are two possible
reasons:

Either (1) the files are not where you have referenced them (have a look in the folder, and make sure
your rule points to that folder, bearing in mind the Project Folder), or (2) the file name is calculating
incorrectly.

We now need to update the rule for the Lever Handle file name to swap in the Ball Handle if that
option is selected.

Model Rules – Replacement Files

8. In the Model Rules, Build the rule for the File Name of the Lever handle.

9. Select IF from the Functions drop down to start the If statement wizard.

10. For the Condition use HandleReturn = “Lever”.

11. Place your cursor inside the Value If Condition Is True input box.

12. Double Click Lever Handle in the Replacements tab on the right side of the Rules Builder
instead of typing it. This ensures that no typing errors are made.

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13. Repeat the steps above, but for the Value If Condition is False, select Ball Handle from
the Replacement Tab.

14. Click Finish to complete the wizard and add the rule to the Rules Builder

Your Rule should look like the following:

Now, if the Lever Option is selected in the Option Group, then a new door assembly will be created
which includes a reference to the existing Lever handle part and if a Ball handle is selected, the Ball
handle part will be swapped into the generated assembly.

15. Close the Project Designer and test the swapping of the file by filling out your Form and
previewing.

Concept: SOLIDWORKS Internal ID

You will notice that the Ball Handle swaps in successfully for the Lever Handle without errors in the
mates. This is because the internal ID of the mates is the same in both models. To achieve this, the
Lever Handle has been copied to be the Ball Handle, and the geometry then changed.

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DriveWorks Solo
Design Automation
for SOLIDWORKS
Lesson 6
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Tables
We can take the replacing of files even further with the ability to drive the replaced file once
swapped in. We will do this by replacing a Circular Window with the Rectangular Window

There are a few tasks that we can do now:

• Use an existing Table in Microsoft Excel to update the Window Combo Box to
include the Circular Window, and reference a picture.

• Add a dynamic picture to the Form, which will update whenever the Window
Combo Box is changed.

• Capture the Circular Windows dimensions.

• Capture the Round Cut Out in the Door.

• Update the rule for the Rectangular Window File Name, and add a rule to
Suppress/Unsuppress the cut out in the Door Assembly.

1. Open up the Project Designer and select the Define Tables task in the Task Explorer.

2. Click the Add button on the Command Bar to add a new Table to your Project.

3. Assign a name for the Table. Call it Windows.

4. Click Finish on the New Table Dialog.

5. Open the Excel File ExternalData.xlsx located in your training folder.

6. Highlight the table on the Sheet Windows and Copy the data onto your Clipboard. Make
sure you include the headers.

7. Select in the Cell A1 in the DriveWorks Table and Paste the data.

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Concept: Tables

DriveWorks Solo tables can either be manually typed in, or have their data copied and pasted from
Excel. It is important to have your data structured as a table, with meaningful column names. This
will become more obvious when we start to reference this table in our rules.

8. Select OK and go back to the Form Design in the Project Designer. Select the Combo Box
for the window.

9. Click in the value for the Items Property in the Property List and click the button to launch
the Rules Builder.

10. Clear the current rule.

We are now going to build a rule that will result in a list of every value in the first column of our
table, except for the header.

11. Click on the arrow below the Functions Button. Select ListAll.

The Function Wizard will show at the bottom of the Rules Builder with two drop downs. The first is a
list of all the tables you have in your Project, at this stage only one, the second will have the column
headers of that table.

Tip:

This is the reason why we mentioned earlier that having meaningful column names is important.

12. Select the name of your table in the first drop down (Windows).

13. Select the first header in the table in the second drop down (Window).

14. Click Finish. DriveWorks Solo will build the rule for you as shown below.

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Note:

The actual arguments passed into the function are the name of the Table, with a DWLookup prefix to
help DriveWorks Solo identify it as a table, and a number which is the column number in the table to
return the list from.

15. In the Help and Diagnostics section at the bottom of the Rules Builder, select the Values
Tab.

The result is the same format as the static value that we had before with the Pipe bar as a separator.

i.e. <Value1>|<Value2>|<Value3>| etc

16. Click OK to apply the rule and close the Rules Builder.

Since we now have a table of values, we can lookup other values in that table based on our selection

17. Add another Picture Box to your Form and call it WindowPicture, click in its File Name
property and Launch the Rules Builder.

Rather than using the File button on the Command Bar, we are going to perform a lookup into our
table and find the corresponding picture for the Window selected in the Combo Box.

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VLookup Function

The function we are going to use is VLookup. Since this is a common function, you will find it by
clicking on the arrow below the Functions button.

There are four arguments of a VLookup:

Lookup This will be the value from the form (Window) and is used for the search

In The table that the data is in

Column The column where the resultant value is located

Match Type True if a nearest match is required, False if an exact search is required

Setting this to True is useful if you have numbers in your first column

Clicking VLookup will activate the Function Wizard for the VLookup function.

1. Click in the Lookup text box to give it the focus. Use the Controls tab on the right and
double click on the Control Name Window. As usual, this will add the control name with
the Return suffix.

2. In the First Combo Box, select the table we want to find the value in. At this point, you
will only have one in there. Select Windows.

3. In the second Combo Box, select the Column header that the result will come from. Select
Picture.

4. In the Match Type combo box, select Exact Match.

Note:

Nearest match would be used if you had a sequence of numbers, say 1,2,3 and 4, and the value you
had to search on was for instance 2.8 in which case the nearest match is 3

You should have the results below.

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5. Click Finish to apply the results from the wizard and click OK to finish building the rule.

6. Switch the Form into Test mode in the Form Designer, and change the Window value to
see the picture update dynamically.

Tip:

Remember, if you can't see the picture, either the paths are wrong, in which case manually edit the
Windows table, or change the mode of your Picture Box to either Zoom or StretchImage.

We are also going to enhance the Form in a number of ways.

We will add a new Form to enter the Window dimensions, but only display it to someone running a
Specification if we have chosen a window at all.

We will only show the dimensions specific to the type of window selected.

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DriveWorks Solo
Design Automation
for SOLIDWORKS
Lesson 7
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Form Navigation

1. Click on the Form Navigation task on the task explorer.

2. Click on the Add Form button to add a new Form to your project. Call the Form Window.

Concept: Form Templates

By default, DriveWorks Solo will create a blank Form when you click Add Form. However, you can
choose to create a Form from a Template.

These templates change size automatically based on the size of the task pane in SOLIDWORKS. They
also create a number of controls instantly for you which may be useful in quickly creating a new
Form for your Project.

3. Click on the Add Decision button to add a decision to your project. Call the decision
WindowReqd

Concept: Connection Points

Form navigation is achieved by dragging the Connection Points from one Form or Decision to
another. The Connection Points are the colored circles that appear either on a Form or Decision, or
near the entry point to the next Form or Decision for an already connected item.

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The decisions have a Green and Red Connection point. Forms have a grey Connection Point.

4. Drag the Connection Point on the end of the exit link of the Details Form, and Drop it onto
the Window Required Decision.

5. Drag the Green Connection Point on the decision and drop it on the Window Form.

6. Drag the Red Connection Point on the decision and drop it on the Finish Node.

7. Drag the Grey Connection Point on the Window Form and drop it on the Finish Node.

8. Your Form Navigation should now look something like this:

Tip:

Click on a Form or Decision to drag it around the screen. Use the alignment buttons on the
Command Bar to organize your navigation.

Tip:

To reposition the arrows that connect the Form Navigation components, left click and hold down the
mouse button on any of the little black blocks .The rectangle will turn into a black square that can
now be dragged around the perimeter of the Form Navigation component.

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The final thing to do on the Form Navigation is to build a rule for the Decision so that DriveWorks
Solo knows which Form to show.

9. Click on the Window Reqd decision.

10. Click the Build button on the Command Bar.

The result of this Rule needs to be either True or False.

If the rule calculates to be true, then the Form with the green link will be shown, if the rule
calculates to be false, then the Form with the red link will show.

If the next Form happens to be Finish, then the specification will be finalized.

We want our rule to be true if either the Rectangular or Circular Window are selected.

11. Type the following in the Rule Editor:

WindowReturn <> "None"

Then if we pick anything other than None, the result will be True, and the Window Form will be
shown.

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DriveWorks Solo
Design Automation
for SOLIDWORKS

Lesson 8
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Enhancing Your Forms

Now that our Form Navigation is complete, we need to add more controls to our forms.

1. Click on the Form Design task on the task explorer.

2. Activate the Details Form in the Form List on the right.

3. We are going to move the window size controls to the Window form.

4. Highlight the Window Height and Window Width boxes by either Ctrl selecting them
both, or by drawing a rectangle around them with your curser.

5. Click the Cut button on the Command Bar (or use the keyboard shortcut Ctrl + X).

6. Switch to the Window Form by selecting it in the Forms List at the top right of the Form
Design.

7. Click the Paste button on the command bar (or use the keyboard shortcut Ctrl + V).

8. Add a new Numeric Text Box to the Windows Form called Diameter.

9. Set a Minimum and Maximum to be 200 and 500 respectively in the Property List.

The final task with the Forms on this section is to hide the Window Width and Window Height
controls when a Circular Window is selected and hide the Diameter control when a Rectangular
window is selected.

Concept: Control Visibility

Controls can be hidden or disabled based on rules. Every Form Control has an Enabled and Visible
property that can be set dynamically

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10. With the Diameter control still selected, click in its Visible property on the Property List.

11. Click the button in the Visible property to launch the Rules Builder.

12. Use the IF function wizard to create the following rule:

Using this rule, the Diameter will only be visible on the Form at run time if the Circular window is
selected. Helping guide a user through configuring a door.

Note:

As this If statement can only result in TRUE or FALSE, the rule can be simplified. The If function can
be removed, and the condition will result in the same value when used on its own.

WindowReturn = “Circular”

13. Click Finish on the Function Wizard to add the rule to the Rule Editor.

14. Click OK to apply the rule.

15. Multi select the other 2 controls on the Form Window Width and Window Height.

Note:

Providing controls have the same properties, you can multi-select them and build rules for a
property that will then be applied to all selected controls.

16. Build a rule for the Visible property as below.

The work for the Form in this section is complete.

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Dynamic Replacement Files

Now that the Form has been updated, we need to make sure that the model updates too.

To do this, we need to capture the Circular Window model, and also capture the round cut out in the
door.

1. Close the Project Designer and click the Save button.

2. Use the Captured Models Section to open the Wooden Door part.

Note:

The Wooden Door part is inside the Door Assembly.

3. Select the suppressed Round Cutout feature in the SOLIDWORKS feature tree.

4. Accept the default name that DriveWorks Solo has used and click Add.

Tip:

Remember that if you have changed the name of a feature or dimension from the original name that
SOLIDWORKS assigns, then DriveWorks Solo will recognize that, and use the changed name.

5. Double click on the sketch for the Round Cutout feature in the SOLIDWORKS Feature
Manager, and capture the diameter dimension. Call it Diameter.

Tip:

Even though the feature is suppressed, you can still capture its sketch dimensions. That said, you
might find it easier to unsuppress it first if the sketch has many dimensions.

6. Open the model Circular Window.SLDPRT which can be found in the same folder as the
other training files using the SOLIDWORKS File Open Menu or Command. Rebuild and Save
the model.

7. Select Click here to capture the current model.

8. Capture the diameter dimension (double click on the feature Boss-Extrude1 to display the
dimension). Use the name Diameter.

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9. Save your Project and then open the Project Designer and activate the Model Rules task.

10. Click the Add button on the Project Designer Command Bar, check the Circular Window
and click OK.

Concept: Component Set

You have now added another Component Set to your Project. DriveWorks Solo allows you to have
as many Component Sets as you want within a Project. You can then choose, based on rules,
whether to create None, One, Many or All of your component sets whenever you fill out your forms.

You can also use any component set as a replacement for any model within your main assembly.

In this case, we will build a rule to replace the rectangular Window with the Circular Window when
we choose Circular from the Window Combo Box.

You will see your new Component Set in the Model Rules Tree.

Note:

If our rules dictate that the Circular Window will be required, then it must have its values calculated
before the main assembly itself. It is therefore important to ensure the Circular Window is above
the Wooden Window and Frame in the tree. It is good practice to position your main assembly/part
at the bottom of the Model Rules Tree.

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The next task for the Circular Window is to update the rules.

11. On the Model Rules task, check the Circular Window in the Model Tree. Making sure any
existing filters have been cleared.

Notice that the rules have already been filled in for the File Name and Relative Path.

We need to update the File Name rule to make sure that if we don't select the Circular Window,
then it won't get created at all.

12. Select the File Name rule for the Circular Window and click the Build button.

13. Clear the existing rule and then use the IF function wizard to create the following rule.

14. Click Finish on the Function Wizard to add the rule to the Rule Editor.

15. Click OK on the Rules Builder to apply the rule.

16. Select the Diameter Dimension in the Rule List and click Build on the Command Bar.

17. Build a rule for the Diameter. This rule will link directly to the Diameter input on the
Window Form.

Next, we need to build a rule for the Round Cutout and Diameter in the Wooden Door Component.

18. Click Refresh in the Command bar of the Model Rules

19. Check the Wooden Door in the Model Tree to show its rules in the Model List.

20. Build a rule for the Round Cutout feature using the following:

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Concept: Features ‘Delete’ keyword

Features will be removed from the model if the rule is calculated to be "Delete".

21. Build a rule for the Diameter. This rule will link directly to the Diameter input on the
Window Form.

The final task is to tell DriveWorks Solo when to swap the Rectangular window for the Circular
window, bearing in mind that we have already built a rule for the Rectangular window to decide
whether to suppress it if no window is selected.

22. Check the Rectangular Window in the Model Tree and with its File Name rule selected in
the Rule List, click Build.

We are going to use a second IF function, nested inside the existing IF function.

23. In the Rule Editor, delete the word Suppress along with the quotes that surround it. Make
sure the curser is still in the position where this word used to be.

24. Click on the arrow below the Functions button on the Rules Builder Command Bar and
select IF to show the IF Statement Wizard.

For the Condition, use:

WindowReturn = "Circular"

For the Value If Condition Is True we want to use the name of the component set to use, if Circular
is selected.

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Concept: Components Tab

You may have noticed that there is a new tab on the Form and Variable Browser called Components.

This gives you an easy way of building a rule to replace one component with another.

25. Once you have clicked in the Value If Condition Is True argument in the Function Wizard,
using the Components Tab, double click on the Circular Window Component.

This adds the text "<Replace>Circular Window" including the quotes.

26. In the Value If Condition Is False argument, type the word "Delete" using the quotes.

Concept: File Name Delete keyword

If a File Name rule evaluates to the text "Delete" then the model will be removed from the new copy
of the assembly it is in.

27. Click Finish on the Function Wizard to add its text to the Rule Editor at the place where
the curser is.

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The resultant rule will be a nested IF function, and with spaces and line breaks added for clarity, will
look like this:

Test your updated rule by running your Forms again. Preview each option to ensure that you get the
results that you expect.

Tip:

If you do not get the results you expect, make sure you look in the Release Reports and Model
Generation reports.

Now add some of the other controls to your form, such as Dynamic Labels. These are handy when
giving onscreen instructions. Building the dynamic Caption Property based on a rule allows you to
give the instruction required dynamically.

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DriveWorks Solo
Design Automation
for SOLIDWORKS

Lesson 9
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Driving Custom Properties

In the first Capture section of this training, we captured some custom properties in our models. We
will now drive these custom properties, including driving Color and Material.

1. In the Project Designer, activate the Model Rules task.

2. Right click on the Wooden Door and Frame and click Select Children.

3. Filter the Rules list by typing custom in the filter box.

Custom Property - Description

1. Select the Description custom property for the Top Door Jamb.

2. Click the Build button on the Command Bar.

We are going to make this text dynamic based on the length of the top door jamb, which is linked to
the Frame Width.

3. Create the rule below. This will build up a descriptive text string.

4. Click OK to apply the rule.

Custom Property - Date

1. Select the Date custom property for the Top Door Jamb.

2. Click the Build button on the Command Bar.

We are going to make this text dynamic based on today's date, which will then be Formatted.

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To do this, we will use the TEXT function

We will also use the function TODAY() which will get today's date.

3. Create a rule that builds up a text string based on today's date.

4. Click OK to apply the rule.

Tip:

It is possible to format dates in lots of different ways. Look in the DriveWorks Solo Help File at the
Text() function for more information.

Custom Property – Color

DriveWorks Solo recognises the custom property DWColor (and DWColour) and uses its value to
drive the color of generated models. The calculated value of the rule needs to be in the format
"255|126|126" where the numbers represent the RGB color.

The spread sheet that we used earlier (ExternalData.xlsx located in your training folder) has a
second sheet with a table of standard colors.

1. Create a new Table in DriveWorks Solo and call it Colors.

2. Open the spreadsheet ExternalData.xlsx.

3. Highlight the table on the Sheet Color and Copy the data onto your Clipboard. Make sure
you include the headers.

4. Paste the data into your new table, remembering to paste into Cell A1.

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5. Select OK on the command bar to save the table.

6. Create a new Combo Box on your Details Form called FrameColor.

7. Build a rule for the Dynamic Items Property by clicking on the button that appears in the
Items Property value box.

8. Use the ListAll function wizard to create a list based on the first column in the table.

9. Click Finish to add the resultant function to the Rule Editor and click OK to apply.

10. Finally, switch back to the Model Rules task in the Task Explorer.

11. Multi-Select the DWColor custom property for the Top Door Jamb and Door Jamb.

12. Click the Build button on the Command Bar.

13. Build a VLookup function rule using its Function Wizard (Found by clicking on the arrow
below the Functions button).

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14. Click Finish to add the result to the Rule Editor.

15. Click OK to apply the rule.

We now need to modify the existing File Name rule for the Top Door Jamb. Earlier on in the training
we created a Variable to represent the color of the Top Door Jamb to give it an Intelligent File Name.
We can now replace this with the color control on the Form.

16. In Model Rules, select Deselect All and clear the filter.

17. Select the Top Door Jamb from the tree and edit the component’s File Name rule.

18. Replace DWVariableFrameColor with FrameColor control.

19. The rule should now look like this:

20. Click OK to apply the rule.

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Custom Property – Material

DriveWorks Solo recognises the custom property DWMaterial and uses its value to drive the material
of the model.

1. Add a List Box to your Details Form using the name DoorMaterial.

2. Build a rule for the Items property of the List Box.

3. Use the List Wizard to build up a list of Materials (found by clicking on the arrow below
the Functions button).

4. Type the values Oak, Pine, Beech, Maple, Mahogany, with each on a new line.

5. Click Finish to add the text to the Rule Editor.

6. Click OK to apply the rule and add the values to the list box.

7. Resize the new Form Control to display all the list items.

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8. Finally, switch back to the Model Rules task in the Task Explorer.

9. Select the DWMaterial custom property for the Wooden Door. You can find this by
selecting all components and using Material in the filter.

10. Click the Build button on the Command Bar.

11. Build a rule using the new list box value.

12. Click OK to apply the rule.

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DriveWorks Solo
Design Automation
for SOLIDWORKS

Lesson 10
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Documents
DriveWorks Solo is shipped with some template documents. One example of this is a quotation.
The quotation is based on XML and creates a HTML document.

1. Open the Project Designer and click on the Documents task.

2. Click the Add button on the Command Bar to add a document to your Project.

3. Select the Quote Document template and give the document a name. Use Quote.

4. Click Finish to add the document to your Project.

The Document View will switch automatically to edit the details of the document. Here you can
build rules to drive the document.

Concept: Document File Name and Relative Path rules

As with models, documents require a File Name rule and a Relative Path rule. Again, as with models,
these have been created for you, although you can change them if required to your desired location.

Documents then have Values that can be driven based on rules.

All these values are automatically mapped through to Variables that are also added when you
created the document.

5. Click the Preview button on the Command Bar. This will open the document in a Browser.

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Notice that there are values in the document that are all driven from Variables. The easiest way of
updating these values is to update the Variables that drive them.

6. Return to the DriveWorks Solo Project Designer and activate Variables by clicking on the
Define Variables task on the Task Explorer.

You will see two new Variable Categories added to your Project, one called Common and one with
the same name as your document (Quote).

7. Click on the Common Category in the Category Tree.

The Variable List will show the Variables in this Category.

In the Common Category you will see Variables for things like Company Name, Company Address (3
lines), Quote Number as well as some dates, and a Customer Contact and Address.

8. Click on the Quote Category in the Category Tree.

In the Category with the same name as your document (Quote) there is some general information
for each line item. If you drill down into this category in the category tree, there is a sub category
called Line Items, which itself contains a category for 50 line items. Each of these sub categories has
4 Variables for Quantity, Description, Discount and Unit Price.

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If you build any of the rules for these variables, they will automatically be updated in the document.

9. Click on the CompanyName Variable either in the Category Tree (in the Common
category) or click the Common category to show its Variables in the list.

10. With the Variable selected, click Build.

11. Change the default text to be your company name and since it is static text, use quotes.

12. Change the StrapLine Variable.

13. Drill down into the Category Tree and build a rule for the Description of Line Item 1 using
Variable QuoteItemDesc1. (This name could be different based on the name you gave the
document.)

The rule we build will use both static text and dynamic text based on Form Control inputs, to build
up a description.

Use the Values, Steps and Drill Down helpers at the bottom of the Rules Builder to assist you in
getting the syntax correct.

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14. Next build a rule for the Item 1 Unit Price using the Variable QuoteItemUnitPrice1.

This name could be different based on the name you gave the document.

At this point, it doesn't matter that our price is in any way accurate.

The rule we build will take into account the overall size of the Door, with a factor for the type of
window used.

Don't use a currency symbol in this rule, just use numbers. The currency symbol is also a Variable,
allowing you to change it based on rules.

We are also going to format the result to always show 2 decimal places using the TEXT function

Start off by multiplying the OpeningHeight and the OpeningWidth, and then divide it by 4000
(arbitrary number)

15. Next, multiply this by a factor based on the type of window selected. There is data in the
table we created for this.

16. Use the Vlookup Function Wizard to assist with this.

17. Click Finish to add the resultant text to the Rule Editor.

Make sure the Cursor is in the correct place in the Rule editor before using the wizard.

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18. Finally, make sure we format the text to show 2 decimal places. To do this, we need to
use the text we have so far as the first argument of the Text function.

Text( <<Text to format>>, <<Format>> )

19. Click on the Function button on the Rules Builder Command Bar. In the dialog that pops
up, select the Text function from the list (use the Filter at the top to reduce the list).

Tip:

All columns will be searched. If you wish to search in one particular column, Name or Description,
then you can specify the name of that column (i.e. name:text). Column names that contain spaces to
separate words should be enclosed within quotes to filter by that column; "Column Name":Criteria

20. Cut and Paste the text from the Rule Editor into the first text box on the Text wizard.

21. Type "0.00" in the second argument, which will format the text to always show 2 decimal
places.

For more information on the formatting options of the Text function, look in the DriveWorks Solo
Help File.

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22. Click Finish to add the text from the wizard into the Rule Editor.

23. Click OK to apply the rule.

24. Change the QuoteItemQty1 to be a static value of 1. (For the adventurous among you,
you could create a spin button on your form, and link this quantity variable to the value of
the spin button).

We will now build the variables for the second line item.

25. Change the Description for Line Item 2 to show text based on the Handle selection by
building a rule for the Variable QuoteItemDesc2.

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26. Change the QuoteItemUnitPrice2 so that it changes dynamically based on your Handle
selection.

27. Change the QuoteItemQty2 to be a static value of 2.

28. Select the Documents task on the Task Explorer and Preview your document in a browser.

29. Close your browser and return to the Project Designer, click OK on the command bar to
apply the changes to the Quote document.

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DriveWorks Solo
Design Automation
for SOLIDWORKS

Lesson 11
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Drawings
We can improve the Drawing that we have already captured, by controlling sheet scale, view
positions, annotation text and much more.

This section covers the capturing and driving of Drawing parameters.

Capturing Drawing Detail

1. With the Project Designer closed, activate the Captured Models section by clicking on its
section header in the capture explorer. If you have no models open in SOLIDWORKS, this
will be already selected.

2. Expand the Captured Models Tree and double click on the Wooden Door and Frame
drawing.

3. Save the Drawing inside SOLIDWORKS.

The drawing is identified by a different icon to the assembly and is a child of the assembly or part
that it is attached to.

Once the drawing has opened, the capture explorer will change to be specific to capturing drawings
with different sections to what are seen with parts and assemblies

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Capture Sheets and Views

The first section is Sheets and Views, which is used to capture the sheets and views that you wish to
control.

Concept: Sheet and View Capture

If you capture a Sheet, you will be able to control its scale based on rules, as well as its state. Sheet
state allows you to Delete a sheet, or rename it based on rules.

If you capture a View, you will be able to control its position on the sheet, its state, which
Configuration to show, and gives the ability to delete and scale it, providing its scale is not linked to
the sheet or its parent view.

1. Capture all of the Sheets and Views by checking them. We are going to control them all.

Notice that an image appears at the top of the Capture Explorer showing the layout of each sheet. If
you select a View in the tree, it will be highlighted in green in the layout picture. This helps to
identify which view you are capturing information against.

You can also resize any of the panes in the Capture Explorer by dragging, as shown in the picture
above.

Information is also displayed about the current size and position of views and sheets, as well as the
Captured information that will be driven based on your rules.

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Notice in the picture that the Scale of Drawing View4 will not be controlled as it is linked to the
sheet scale.

Capture Annotation text

1. Activate the Annotation Text section by clicking on its section header.

Capturing annotation text allows you to drive text on your Drawing based on rules. As with model
dimensions, we capture annotation text by selecting it in the Drawing, and assigning a meaningful
name to it in DriveWorks Solo.

2. Switch the Drawing to view Sheet 2 in SOLIDWORKS.

3. Select the text on Sheet 2 which currently reads Door-DoorSize.

4. In DriveWorks Solo, enter a meaningful name. Use Door Text.

5. Click Add to capture the Annotation text.

6. Select the text on Sheet 2 which currently reads Frame-FrameSize.

7. In DriveWorks Solo, enter a meaningful name. Use Frame Text.

8. Click Add to capture the Annotation text.

9. Select the text on Sheet 2 which currently reads ContainsWindowReqd.

10. In DriveWorks Solo, enter a meaningful name. Use Window Text.

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11. Click Add to capture the Annotation text.

You can also capture annotation position. Doing so enables you to control the dimension to the left,
top, right and bottom. Information on the rules required to do this can be found in the Help File.

Capture Annotation Positions

1. Activate the Annotation Positions section by clicking on its section header.

When you capture annotation positions around a view, they are placed back in the same relative
position to their location during capture.

You can link the positions to the top or bottom and then either the left or the right.

2. In the Capture Explorer, on the Annotation Positions section, select Drawing View4 in the
tree.

The selected view will be highlighted in Green in the preview, and the view will be selected in
SOLIDWORKS. If the Drawing is not showing the correct sheet, then this will be activated
automatically.

3. In SOLIDWORKS, drag-select around the dimension and balloons on the left of the view.

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This will highlight the dimensions and balloons in SOLIDWORKS to the left of the view.

4. Check the Left Checkbox.

5. Click Apply.

The selected dimensions will be added to the tree. Without the need for Rules, these dimensions
will be placed back in these relative positions when a new drawing is created, regardless of the size
of the new model and view.

We will now do the same for the Top, Right and Bottom.

Tip:

SOLIDWORKS does not always update the selected items collection when selecting balloons. If you
<Control>Select a dimension to select it, and then <Control>Deselect the same dimension to
deselect it, then SOLIDWORKS will update its selected items collection allowing you to capture
Balloons only.

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6. In SOLIDWORKS, drag-select around the balloons on the top of the view.

This will highlight the balloons in SOLIDWORKS to the top of the view.

7. Check the Top Checkbox.

8. Click Apply.

Notice that the Left Checkbox has changed to be a partially selected state. This is because some of
the currently selected annotations are already captured to the left, and some of the currently
selected annotations are not.

Tip:

When drawing the fence in SOLIDWORKS, if you draw from Top Left to Bottom Right, it selects
everything that is inside the fence. If you select from Bottom Right to Top Left, it selects everything
that is inside the fence AND everything that crosses the fence.

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9. In SOLIDWORKS, draw a fence around the balloons on the right of the view. Again, you
may need to <Control>Select and <Control>Deselect a dimension to get SOLIDWORKS to
update its selected items collection.

10. Check the Right Checkbox.

11. Click Apply

12. In SOLIDWORKS, select the dimension at the bottom of the view.

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13. Check the Bottom Checkbox.

14. Click Apply.

You can use any selection method you choose to select annotations, including single click select, and
multi click select using the <Control> key.

If you move any dimensions around on the sheet after capture, simply click the Update Positions
button.

You can also deselect Captured annotations, by selecting them in SOLIDWORKS, and checking the
appropriate position check box until it is the state you require.

There is no right or wrong position to capture an annotations position too. Think about how your
view will change when your model changes, this should give you a good idea as to which side you
want the annotation to be ‘locked’ too. Also remember that an annotation can be captured to
multiple sides of a view.

Capturing Layers
DriveWorks Solo allows you to control the visibility of Layers on your Drawing.

1. Activate the Layers section by clicking on its header in the Capture Explorer.

The list will then show the current Layers in your Drawing.

To Capture a Layer, check it in the list. For the purposes of this training, we are going to capture the
Layer Description text. The annotations you captured earlier for the Door, Frame and Window Text
are the only items on this layer. Using a rule to hide the layer will therefore hide these annotations.

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2. Check the layer Description Text in the list.

Capturing Custom Properties

DriveWorks Solo allows you to control Drawing Custom Properties so that you can drive their text
based on rules.

1. Activate the Custom Properties section by clicking on its section header.

The Custom Properties Section will show you all of the Custom Properties that are currently in your
Drawing.

In this particular Drawing, the Custom Property PART NO. is linked to the Drawing Number field in
the Drawings border.

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2. Use the filter box at the top to filter the custom properties by typing in the word part.

3. Check the PART NO. custom property to capture it.

Note:

As with Model Custom Properties, you can add new Custom Properties to your Drawing by typing in
a new Custom Property Name and clicking Create.

Capturing File Formats

DriveWorks Solo allows you to export your driven drawing to different file formats.

1. Activate the File Formats section by clicking on its header.

2. Select Yes in the Captured PDF pull down.

Each time you create a new version of this drawing, you will now get a PDF version automatically.

Concept: Capture With Rules

The With Rules capture option will allow you to specify additional parameters for each file format.

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Building Rules for the Drawing

The captured information in the drawing can now have rules built to control their values.

1. Save your project.

2. Open the Project Designer by clicking on the button on the DriveWorks Solo Command
Bar.

3. Click on the Model Rules task in the Task explorer and click the Refresh button in the
command bar and make sure the filter field is clear.

4. The Tree shows the captured models. Drill down to the appropriate model to see its
drawing.

5. Select the drawing Wooden Door and Frame Drawing in the tree. The drawings again
have a different icon to the parts and assemblies.

The rules for this drawing now appear in the rules list, a preview of the drawing and information will
show at the bottom, depending on which sheet/view you select.

The bottom section is for information only, and will allow you to see which view you are working on
using the preview, and to see the current information about each sheet and view.

The Model rules also have a filter box to assist you when looking for rules.

Notice that rules have automatically been created for the File Name and Relative Path just as they
were for Parts and Assemblies

Layer Rules
We will start by building a rule for the captured Layer. We may want a Check Box on our form, to let
the user decide whether or not to show that layer.

1. Add a Check Box control to the Details Form called ShowDrawingNotes.

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2. Go back to Model Rules, select the rule for the Description Text layer and click Build.

3. Build an IF statement rule so that if the ShowDrawingNotes Check Box is checked, then
the Layer will be visible, and if not, it will be hidden.

Annotation Text Rules

Annotation text is controlled by building a rule that will be calculated to be a text string.

1. Select the Door Text rule in the Model Rules List.

2. Click Build.

3. Build a rule that will describe the door.

4. Select the Frame Text rule in the Model Rules List.

5. Click Build.

6. Build a rule that will describe the frame.

7. Select the Window Text rule in the Model Rules List.

8. Click Build.

9. Build a rule that will describe the window.

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If there is no window, then we should delete the note. The rule also needs to take account the type
of window. We will use a nested IF function.

Custom Property Rules

Custom Properties are controlled by building a rule that will be calculated to be a text string.

10. Select the PARTNO. rule in the Model Rules List.

11. Click Build to build a rule for the PARTNO. Custom Property.

Build a rule for the part number. In this case we are going to build up a text string based on some of
the items that will change.

Notice the use of the Left function to return the first character from the Window and Lever
selections.

Sheet Rules

12. Unselect the Wooden Door and Frame Drawing from the Model Tree.

13. Expand the Wooden Door and Frame Drawing and select Sheet1 and Sheet2

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14. Select the Sheet1-Sheet State rule in the Model Rules List.

15. Click Build.

For sheet state, you can build a rule that will evaluate to the result "Delete" if you want to delete the
sheet, or to some other text value if you wish to rename the sheet.

Renaming sheets can be useful as DriveWorks Solo will automatically export a DWG or DXF file based
on that sheet if the name is changed to either of those.

We will build a static rule that will automatically export a DWG file of sheet1 each time a new
drawing is created.

16. Create a static text rule that will change the name of the sheet.

The only other items we are going to build for the sheets at this point are the scale values.

Concept: Scale Numerator and Denominator

DriveWorks Solo allows you to build a rule for both the Scale Numerator and the Scale Denominator.
If the Numerator is greater than the Denominator, then the scale will be greater than 1:1 and vice
versa.

17. Build a rule for the Scale Numerator of both Sheet1 and Sheet2 to be a static value of 1.

Tip

You could multi select these 2 rules to build the rule for both at the same time.

We now need to calculate the scale Denominator. In this case, because of the orientation and types
of views that we have on our sheets, the only dimension that will significantly influence the required
scale of the sheet is the Opening Height.

Your Sheet scale rules may need to take into account multiple dimensions if the product you are
automating has more complex geometry.

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We will use a simple rule, calculated from the basis that:-

NewScale = NewHeight

ExistingScale ExistingHeight

Transposed for the New Scale, we get:

NewScale = ( NewHeight / ExistingHeight ) * ExistingScale

And then to make sure that we only get a whole number, we can add the roundup function with an
argument of Zero decimal places.

NewScale = ROUNDUP( ( NewHeight / ExistingHeight ) * ExistingScale , 0 )

18. Using this, build a rule for the Scale Denominator of both sheets.

Where 2245 is the current size in the model for the opening height, 20 is the current scale.

Tip:

This will possibly result in a non-standard sheet scale. If you want to use standard sheet scales,
create a table of allowable sheet denominators, and then use the VLOOKUP function to find the
nearest value, both looking up in, and returning from, the first column.

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View Rules
Since the View scales are linked to either the sheet, or the parent view scale, we don't need to build
rules for these for this drawing. If we did, we would build them in exactly the same way as the Sheet
scale.

Concept: View Delete keyword

The View state rules can be built to delete a view, if the result of the rule evaluates to "Delete".

We now need to build rules to position the views on our drawing. When a drawing gets rescaled,
the views can be moved to new locations. Building these rules ensures that the views are positioned
exactly where we want them.

These rules will control the Top Left position of each view measured in the Drawing Units from the
bottom left hand corner of the sheet.

You can drive your view positions to be exactly where you want them, although in this case, we are
going to build rules to position them back to their original locations on the sheet.

The original locations can be found by clicking on each view in turn in the bottom panel of the Model
Rules List and noting the Top and Left positions in the Information Panel.

1. Build the rules for all of the View Positions to locate them back to their original locations.

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Notice that position has been typed into the filter box to limit the rules to the view positions, and
also that approximate values have been entered compared with the exact current locations of the
views.

Tip:

If a view is aligned to another View in SOLIDWORKS, then DriveWorks Solo will ignore driving the
position in the alignment direction.

The work on Drawings for this training is complete.

Run your Project a few times to ensure that all of the rules are correct and that you are generating
the desired results. If you are not generating the results that you expected, re-visit and amend your
rules accordingly.

This also concludes this DriveWorks Solo Training course. If you would like to further your learning,
check out the DriveWorks Community (https://hub.driveworks.co.uk/). There you will find more
information on:

- DriveWorks Solo – How-To Videos

- DriveWorks Solo – Tutorials
- DriveWorks Solo Certification

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Appendix
Preparing Your Models for Automation
The models that were provided for you during this evaluation were created with automation using
DriveWorks. They therefore have no design tables, or in-context design, and have been mated
together on pre-defined planes.

When DriveWorks creates new model sets based on the masters, it is copying files and then re-
referencing any associated files.

It is therefore wise to construct the models and create mates knowing what is to be driven.

For instance, if you mate parts in an assembly based on one of its features, and then delete that
feature based on a rule, the mate will error in the new clone.

It is therefore important to understand just how models will be driven. It is also important to be
able to understand the design logic, especially when building and testing the rules. If in-context
design is used, along with design tables and/or equations, and then DriveWorks is also used to drive
dimensions, features and custom properties, correcting any unexpected model results can be hard
work, as it’s difficult to know where to look first to resolve the issue.

In-context Design
Be careful with in-context design when drilling down more than one level. DriveWorks is fine with
one level of in-context design, but because DriveWorks is creating new files based on the masters,
you need to be careful to ensure that the correct model is referenced at all times.

Therefore do not have a Part in an assembly that is modelled up to a face on a different part in the
same assembly, as the references will not update correctly when new clones are created.

DriveWorks will also not update references if a Part is in a sub assembly, which is in an assembly,
and the part is modelled in-context of the top level assembly. Stick to one level only.

If multi-level in-context design is insisted upon, then have sketches or planes in the sub assembly
that are in-context with the assembly, and then drive the Part from the sub assembly.

Part Equations
Using part equations is fine, although DriveWorks will only perform the rebuild operation once and
after it has driven dimensions, features and custom properties. If the equations are in the wrong
order, subsequent manual rebuilds may be required.

That said, there is an argument to say that if you are controlling dimensions from DriveWorks based
on rules, there is little need to use equations.

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Assembly Equations
Avoid using assembly equations. They can cause unexpected results in the resulting files.

Configurations
DriveWorks can use rules to select an existing configuration to use, but it does not create new
configurations. Also when it is driving a dimension or feature, it will do this for all configurations,
unless the feature or dimension is configuration specific, then it will only be driven in that
configuration.

DriveWorks File Formats

A DriveWorks Solo project consists of two files. They have the same name, but a different extension.
The file name of each is the name of the project, and the extensions are:

• ProjectName.drivegroup
• ProjectName.driveprojx

Both these files are located in the folder selected to create the project in.

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Useful Information
The DriveWorks Solo Help File is an invaluable source of information. Press F1 on your keyboard, or
click the question mark button while in the product.

The online Help version is continually updated with new articles and represents the version that will
be incorporated into the next service pack of DriveWorks.

You can view the Help File online at http://help.driveworkssolo.com/

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Glossary
A
Adding Captured Models to the Project Designer ................................................................... 52
Alignment Guides..................................................................................................................... 37
Associated Drawings ................................................................................................................ 24
Asterisk character .................................................................................................................... 74

C
Capture With Rules ................................................................................................................ 140
Captured Models ..................................................................................................................... 18
Capturing.................................................................................................................................. 15
Combo Box ............................................................................................................................... 39
Command Bar Overflow........................................................................................................... 35
Component Set ...................................................................................................................... 104
Components Tab .................................................................................................................... 107
Configurations .......................................................................................................................... 70
Connection Points .................................................................................................................... 95
Control and Variable Double Clicking ...................................................................................... 48
Control Properties.................................................................................................................... 36
Control Visibility ..................................................................................................................... 101
Custom Property Special Names.............................................................................................. 23

D
Design Intent ............................................................................................................................ 19
Document File Name and Relative Path rules ....................................................................... 119

F
Features Delete keyword ....................................................................................................... 106
File Name and Relative Path .................................................................................................... 54
File Name Delete keyword ..................................................................................................... 107
File Name Rule ......................................................................................................................... 69
Form Controls .......................................................................................................................... 36
Form Design ............................................................................................................................. 34
Form Navigation....................................................................................................................... 34

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G
Group Controls ......................................................................................................................... 42

H
Help links .................................................................................................................................. 12

I
Input Validation ....................................................................................................................... 13

L
Lists .......................................................................................................................................... 39

N
Navigation Decision ................................................................................................................. 35
Nested IF Functions.................................................................................................................. 71

O
Opening DriveWorks Solo ........................................................................................................ 11

P
Preview Button ........................................................................................................................ 62

Q
Quick Text ................................................................................................................................ 59

R
Relative Path rule ..................................................................................................................... 69
Rules Builder Diagnostics ......................................................................................................... 50

S
Scale Numerator and Denominator ....................................................................................... 143
Sheet and View Capture ........................................................................................................ 130
SolidWorks Internal ID ............................................................................................................. 83
SolidWorks Naming Convention .............................................................................................. 19
Static and Dynamic Values ....................................................................................................... 38
String concatenation ................................................................................................................ 74

T
Tables ....................................................................................................................................... 88

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U
Unique file names .................................................................................................................... 75

V
Variable Categories .................................................................................................................. 47
View Delete keyword ............................................................................................................. 144

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