SOLIDWORKS MBD Demonstration V1.1
Ian Pilkington – Product Marketing
SOLIDWORKS MBD Demo Script
SOLIDWORKS MBD Demonstration V1.1
Ian Pilkington – Product Marketing
Pre-Requisites – Quick checklist.
1. Ensure SOLIDWORKS 2015 SP1.1 or later is installed along with eDrawings. NOTE: SOLIDWORKS
MBD will be officially released with SP2.0. Some functionality will be limited until full release.
2. Enable the MBD Toolbar.
3. Copy the two template folders ‘A4 Assembly Landscape’ and ‘A4 Part Landscape’ into the themes
directory - ‘C:\Program Files\SOLIDWORKS Corp\SOLIDWORKS\data\themes’
4. If you wish to make changes to the PDF Templates, you need to have write access to ‘C:\Program
Files\SOLIDWORKS Corp\SOLIDWORKS\data\themes’ and subsequent folders.
5. Copy ‘Default Notes.sldnotestl’ from the Default Notes folder to the annotations folder in your
design library (e.g. C:\ProgramData\SOLIDWORKS\SOLIDWORKS 2015\design
library\annotations).
6. Ensure the latest version of Adobe Reader is installed.
7. Enable ‘Rotate around Scene Floor’
Optional but recommended
1. Enable the Configuration Switcher Toolbar. This allows you to switch to the different configurations
from a drop down box
2. Add the ‘Normal To’ command ( ) to the Heads-Up-Display.
3. Add Location Dimension and Size Dimension to the in-context graphics window. Alternatively add
these to the ‘S’ key. Either method reduces mouse movement when creating dimensions.
SOLIDWORKS MBD Demonstration V1.1
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4. Turn off Instant 3D. This prevents the dimension edit box popping up when you select feature
dimensions.
SOLIDWORKS MBD Demonstration V1.1
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Introduction
The complete demo movie, the movie transcript and this script are in the Movie folder – MBD Demo
V1.0.mp4, MBD Demo movie transcript 1.0 & MBD Demo Script V1.1.PDF.
The demo is based on an underwater camera manufactured by Watershot. The main portion of the demo
focusses on the GEAR PLATE.SLDPRT part and the creation of several 3D Views which contain important
PMI (Product Manufacturing Information). These views ultimately are published into both eDrawings
and PDF format.
Additionally, the top level assembly - GEAR ASSEMBLY.SLDASM – contains some 3D Views which act as
an introduction to the product and are also later published to PDF.
Please refer to the movie to learn the demo. The following notes will help you understand particular steps
in the demo.
Note: Completed files for GEAR PLATE.SLDPRT, GEAR ASSEMBLY.SLDASM and the final PDF files are
located in the ‘Completed Files’ folder.
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Part 1 – Demo introduction 0:00 to 1:30
This is an opportunity to set the scene of the demo. The movie shows the completed GEAR PLATE part
with 3D Views. It then goes on to show the operation of the assembly. The messaging here is that
SOLIDWORKS MBD lets you detail your models quickly and easily without the need to create an
additional 2D drawing. 2D drawings are prone to interpretation errors whereas MBD lets you work
directly on the model and create manufacturing information that is very easy to digest and understand.
Part 2 – GEAR PLATE part – Adding standard Notes 1:30 to 2:00
There are two existing 3D Views in the model. The ‘ISO – ALL DIMS’ view shows all annotations
excluding notes. The ‘OVERVIEW’ view excludes all annotation except notes.
Note: When you drag the ‘Default Notes’ into the graphics window be aware that when you first
spin the model or select the text, the note may fly off the screen. This is a known issue that will be
addressed before release. You can optionally have this note already created to save time.
Part 3 – Auto Dimension of GEAR PLATE part. – 2:00 to 2:44
Auto Dimension is a great way to create default datums and initial dimensions. Make sure you switch to
the ‘ISO – ALL DIMS’ 3D View before performing the Auto Dimension.
Note: as part of specifying the tertiary datum, you create a compound surface. This tells SOLIDWORKS
that the hole is continuous i.e. drilled in one operation.
Tip: After selecting the flat surface for the primary datum you can click the right mouse button to
advance to selection of the secondary surface (and similarly to move from secondary to tertiary).
Part 4 – Highlighting Geometry – 2:44 to 3:00
When creating DimXpert dimensions, SOLIDWORKS gives you the opportunity to show which surfaces
are fully defined (green) or not.
SOLIDWORKS also lets you change the display in the DimXpert manager to show an annotation based
view. This is simpler to explain to most users and nicely shows the ability to cross highlight dimensions,
datums and geometric tolerances – a big advantage over 2D drawings.
Part 5 – Creating the Top View - 3:00 to 3:40
Activate and Orient the ‘TOP’ annotation view. This ensures you have both the correct orientation on
screen and that and dimensions you create will (mostly) be placed on that plane.
For the first part of the demo, you manually recreate the basic dimensions.
Info: Basic dimensions can be considered to be absolute. That is, they have no tolerance. Basic dimensions
describe the theoretically perfect location of a feature. The tolerance of the feature is controlled by a
SOLIDWORKS MBD Demonstration V1.1
Ian Pilkington – Product Marketing
geometric tolerance. In this case (and for all the holes in this demo) these are positional tolerances that
simply say “the center of this hole can be within a circle of diameter 0.5mm around the theoretical center”
Two of the basic dimensions (the 3 and 4 dimensions) appear on other annotation planes. You move
these onto the TOP view by highlighting the dimensions and pressing the ‘ key (apostrophe).
Info: Capturing 3D Views is very straightforward and powerful, although there are some things to
remember. This will really help you understand the functionality.
3D Views will snapshot;
1. The orientation
2. The annotation plane visibility (you can include/exclude whichever you wish)
3. Visibility of Feature Dims, Reference Dims and Dim Expert Dims (RMB over the Annotations folder to see if
these are turned on or off)
4. Reference Geometry visibility such as axes, points etc.
5. Section visibility
6. Model display (Shaded, wireframe etc)
7. Configurations
8. Display States
Part 6 – Creating the Front View – 3:40 to 4:01
Make sure to Activate and Orient the FRONT annotation view. The rest is straightforward. The TOP
annotation plane is excluded from the 3D View but it could be left in if you wish.
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Part 7 – Adding the information for the radial hole pattern – 4:01 to 4:54
In this step you auto dimension the hole pattern but use a plus/minus scheme with a polar option.
This ensures the holes are dimensioned by angle rather that with X&Y coordinates.
Creating new annotation planes is really easy and allows you to dynamically add which annotations you
want to move onto that plane as part of the creation. (4:37 to 4:47)
This then allows you to capture a 3D View that just shows this annotation plane.
This technique is really useful when you want to document multiple manufacturing operations that are in
the same orientation. In a 2D drawing you would create multiple views in much the same way but
without the ease of understanding downstream.
Part 8 – The Right View – 5:05 to 6:46
This section shows how to manually dimension components in SOLIDWORKS MBD. It’s also set up to
show the automatic update later in the demo when you change to a new configuration.
The first dimension makes use of the compound plane capability. This ensure that SOLIDWORKS
recognizes the whole surface as one geometry reference and highlights accordingly. The other three
dimensions are very straightforward – notice that the Location Dimension tool stays active so you do
not need to press the icon again for each one.
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The intersection dimension allows you to dimension to the intersection of two surfaces. To select an
intersection select the first surface then select the intersection icon in the pop up toolbar. Now, select the
second surface and the green tick to finish. Repeat this for the other intersection.
By default, the created dimension is normal to the angled surface. DimXpert allows you to change this to
horizontal, vertical or normal to a user defined reference.
Size dimensions relate to features like holes, fillets and chamfers. SOLIDWORKS dimensions these as per
the DimXpert settings under document properties.
Part 9 – Re-using feature/sketch dimensions – 6:46 to 7:20
This section shows how you can reuse dimensions – something that is important to show. In many cases
the design intent will not necessarily match the way features are dimensioned, but being able to display
existing dimensions is high on the list of customer requirements.
In this model, all the feature dimensions have been moved to the ‘Unassigned Items’ annotation view to
make things simpler.
By default in SOLIDWORKS, all the feature dimensions are tuned off (RMB in the Annotation folder).
The process for this step is;
1. Activate and Reorient to Left annotation view
2. Turn on Feature Dimensions
3. Show the Unassigned Items annotation view (all the feature dims will now be visible)
4. Select the required dimensions. (Tip: Turn off Instant 3D to prevent the dimension value dialogue popping
up)
5. Flip the dimensions into the Left annotation view (press the ‘ key and select Left)
6. Hide the Unassigned and Right annotation views
7. Hide DimXpert dimensions under the Annotation folder (this prevents dimensions created in the next step
from being visible in this view)
8. Capture the 3D View
SOLIDWORKS MBD Demonstration V1.1
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Part 10 – Creating a section view - 7:20 to 8:32
This section shows how to create views with sections along with the ability to create dimension schemes
for hole patterns quickly and easily.
After creating the section, orient back to the left view and capture the 3D View. It is recommended to add
the ‘Normal To’ command to the heads-up-display as use this. Alternatively, use mouse gestures.
Being able to set up these section views quickly and easily offers big advantages over the cumbersome
way of creating projection/detailed/section views.
Showing the options highlights how flexible SOLIDWORKS is and how it conforms to detailing standards
such as ISO or ASME 14.5. This also explains where the default tolerance values come from.
Setting these values ensure that companies adhere to standards and design intent is passed to
manufacturing in a consistent manner.
When creating the geometric (positional) tolerance, make sure the size dimension is pre-selected. This
ensures that the feature control frame (the name for the box with the tolerance information) appears
correctly below the dimension.
Make sure to select the diameter and maximum material condition options so the location dimensions are
created correctly.
Optional:
If you enter an incorrect value into one of the reference boxes (Datum Z in this case), SOLIDWORKS will
highlight this as an error. This shows that SOLIDWORKS is creating intelligent manufacturing information
– not just a nice drawing!
SOLIDWORKS MBD Demonstration V1.1
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Part 11 – Dynamic Annotation View – 8:32 to 8:53
When Dynamic Annotation View ( ) is active only dimensions that lie on a plane within about 12
degrees of the view normal are visible. Annotations fade in and out as you rotate the model. This also
means that items on the Front plane WILL NOT be visible if you are oriented in a Rear view.
Under the Annotation menu (RMB on Annotation folder) there is an option to include all views when
using Dynamic Annotation View.
This can be very useful but be careful that this will also make the default notes created in Part 2 visible.
You may find that these notes jump around on screen.
Part 12 – Configurations – 8:53 to 9:37
Ensure that the RIGHT 3D View is active before switching the configuration.
When copying the dimensioning scheme SOLIDWORKS effectively recreates all of the dimensions you
created earlier. The redundant dimensions are visible on screen and also in the DimXpert Manager.
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Part 13 – eDrawings – 9:37 to 10:04
IMPORTANT NOTE: Functionality in SP1.1 is limited for now.
Have the Version 2 3D View active and just publish the Default and Version 2 configurations.
Highlight the 3D View thumbnails but DO NOT select any of them.
Show the cross highlighting of surfaces when selecting any dimension.
Part 14 – PDF Template Editor – 10:04 to 10:57
This is all set up in advance so you do not need to do anything tricky.
Templates ensure that the resulting PDF’s follow company standards and are repeatable – just like
drawing templates.
If you wish to create some customizations to your demo bear the following in mind;
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1. You will need to have write access to C:\Program Files\SOLIDWORKS Corp\SOLIDWORKS\data\themes in
order to save changes or new templates. The templates take the form of a folder containing the necessary
information.
2. You can easily insert a custom image to personalize the demo template.
3. For information there are four types of text field when you create a text box.
a. Text Field. This will prompt the user to enter a value during the PDF export process in
SOLIDWORKS.
b. Template Text Field. This is just a simple text box (for example the standard notes).
c. Custom Property Field. This will map a custom property from SOLIDWORKS such as Material or
PartNo.
d. PDF Form Field. This will become an editable field within the PDF.
4. Aligning text boxes can be tricky. Template Text Fields tend to align the text toward the top of the text box
whereas Custom Property Fields tend to align at the center.
Part 15 – PDF Publishing and Viewing – 10:57 to 11:55
IMPORTANT! In SP1.1 there is a limitation that only allows the current configuration to pass
DimXpert dimensions into the PDF.
Contrary to the video, switch to the ‘ISO – ALL DIMS’ view before selecting ‘Publish to PDF’. This
will mean, however, that the Version 2 view will not show any dimensions.
This will be fixed before official release.
After selecting ‘Publish to PDF’ choose the ‘A4 Part Landscape’ template.
When choosing which views to output, select all views ( ) and then deselect ‘Current Model View’
& ‘Overview’;
SOLIDWORKS MBD Demonstration V1.1
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Make sure ‘View PDF after saving’ is ticked;
The export process takes a few seconds and the PDF should appear on screen.
The PDF should contain a blue box which highlights the PDF form field – where you can enter some
comments.
As the ‘Version 2’ view contains no dimensions, select the ‘Right’ view to show the cross highlighting of
dimensions.
Tip: Sometimes selecting the dimension text does not immediately highlight the geometry. Select the
witness or leader lines instead.
Tip: Manipulating the model;
1. Spin the model using the left mouse button (LMB)
2. Zoom using the mouse thumb wheel or the right mouse button (RMB)
3. Pan using ctrl+ LMB or by holding both LMB + RMB
When the number of 3D Views exceeds seven, the views overflow to the right. To see these views select
the arrows as below;
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PDF settings: Use the following 3D settings in Adobe Reader;
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Part 16 – Annotating the assembly - 11:55 to 13:00
When creating the dimension, make sure to select a planar surface rather than a vertex. Otherwise,
SOLIDWORKS will ask to create a new annotation plane to define the annotation placement rather than
place it on the Right annotation plane.
Ensure that sketches are turned on in order to see the point at the center of the gear axis below.
When publishing the PDF, use the ‘A4 Assembly Landscape’ template and select all views to output
except ‘Current Model View’.
SOLIDWORKS MBD Demonstration V1.1
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Tip: To have the BOM published into the PDF, you need to create a BOM Table in the assembly. In
this example the table is hidden but you can unhide it in the ‘Tables’ folder.
Part 17 – Assembly PDF – 13:00 to finish
The main feature here is the ability to see and cross highlight components in the BOM table.
Tip: Once you select an item in the table, it will cross highlight in the graphics window in green.
The whole view then becomes transparent. To revert to solid parts, double click in the graphics
window.
Tip: You can see the model tree by selecting the model tree icon;
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Other Useful Information:
1. If you need to delete all of the DimXpert information without reloading the part, use the ‘Delete’
command from the RMB in the DimXpert manager.
2. If you wish to window select many dimensions/callouts, use the selection filter from the RMB on the
screen (new in 2015).
SOLIDWORKS MBD Demonstration V1.1
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3. When hiding/showing/deleting multiple annotation views in the annotations folder, you can
Shift+Select multiple views to save time.
4.
