How to prepare and import SOLIDWORKS Parts and Assemblies

We use the CAD-Line dialog-box | Solids tab to import SOLIDWORKS Part and Assembly documents.


The correct 'Type-Library' file must be in the MechDesigner installation directory before you can import documents from SOLIDWORKS.

In MD14 and later, the Type-Library files are installed automatically. If you use change to a different SOLIDWORKS release, then MechDesigner automatically switches to the same Type-Library.

To check the Type-Library, see the Help menu > About > Type Library tab.

Coordinate Systems in SOLIDWORKS and MechDesigner

This CAD-Line is automatically added with the Added-Part.

This CAD-Line is automatically added with the Added-Part.

CAD-Lines and Coordinate Systems in MechDesigner

CAD-Lines are along the centre of all Added-Parts. Add Cad-Lines with the Part-Editor, at any position, even over/above the CAD-Line along the centre of the Part.


Origin of the Coordinate System: the start-Point of the CAD-Line is always the Origin
+X–axis of the Coordinate System: is along the CAD-Line, from its start-Point to end-Point
+Y–axis of the Coordinate System: is at +90º to the +Xaxis
The +X and +Yaxes are coplanar with the Mechanism Plane.
The +Zaxis is perpendicular[] to the Mechanism Plane. In the Front-View of the Mechanism-Editor, the +Z–axis is towards you, the viewer.

The image above shows the CAD-Line that is added automatically from the start-Point to the end-Point of an Added-Part.



We must add a Coordinate System to the SolidWorks model. To help, I:

1.Add a new Plane 1s-red

It becomes the XY-Plane of the new Coordinate System.

2.Add a new Sketch2s to the new Plane1s-red:

Add two perpendicular[⊥] construction lines, that intersect.

The directions of the Lines become the +X and the +Y–axes of the Coordinate System.
The intersection of the Lines becomes the Origin of the Coordinate System.
The perpendicular[⊥] to the Plane becomes the +Z–axis of the Coordinate System - using the Right-Hand Rule for Coordinate Systems.
Add Coordinate Syastem dialog in SOLIDWORKS

Add Coordinate Syastem dialog in SOLIDWORKS

3.Use SW > Insert menu > Coordinate System to add a new Coordinate System 3s
a.Click the Point at the intersection of the two Lines as the Origin
b.Click the construction line that you want to become the +X-axis
c.Click the construction line that you want to become the +Y–axis.

The +Z–axis automatically becomes normal to the Plane defined by the +X and +Y–axes and the Right-Hand-Rule.

The +Z–axis is towards you, the same direction as the +Z–axis of the Mechanism-Editor in MechDesigner.

Procedures to import SOLIDWORKS Documents

tog_minusProcedure 1: Import one SOLIDWORKS Part onto one CAD-Line


Add a new Coordinate System to the document in SOLIDWORKS (Refer to the images above):

Step 1: SOLIDWORKS > Insert menu > Add Reference Geometry > Reference Plane

The new Plane becomes coplanar with the Mechanism Plane and Part Plane in MechDesigner.

Frequently, I offset the new Plane to be 'in front' of the Solid body in SOLIDWORKS

Then, the Solid will display 'behind' the Mechanism Plane in MechDesigner. The kinematic elements will show and they will be easy to edit.

Step 2: SOLIDWORKS > Tools menu > Sketch Entities > Line (Construction Lines)

Draw two construction lines on the new Plane. It is easy to edit the sketch later, if necessary.

Thus, add constraints/relations to make the lines:

Make one Line align with the +Xaxis of the Coordinate System (this will be along the CAD-Line) and the other Line along the +Y-axis
Make the Lines intersect at the position you want to become coincident with start-Point and origin of the CAD-Line

Step 3: SOLIDWORKS > Insert menu > Add Reference Geometry menu > Reference Coordinate System

In the SOLIDWORKS Add Coordinate System dialog selection-boxes:

Origin: Select the intersection of the new construction lines.
X–axis and Y–axis: Select the construction lines as the +X–axis and +Y–axis.

SOLIDWORKS will add the +Z–axis with the Right-Hand-Rule.


Step 1: To show the Solid you will import from SOLIDWORKS

Use Tools menu( or toolbar) > Show model in Mechanism.

Step 2: MechDesigner > Open CAD-Line dialog-box.

[Click the CAD-Line onto which you want to import the SOLIDWORKS® Part. In the Selection-Window, right-click the CAD-Line, in the contextual-menu click 'Edit element']

In the CAD-Line dialog-box:

1.Click the SOLIDWORKS tab
2.Click the 'Model Import from SOLIDWORKS' separator
3.Click the Read button.

Wait until the SOLIDWORKS Part, Configuration and Coordinate System show in the boxes below.

For a large model, this may take many seconds.

4.Click the Import Model from SOLIDWORKS button (at the bottom of this separator)

Wait until the Import Model from SOLIDWORKS button 'releases' and its action is complete.

You may need to click 'Import Model from SOLIDWORKS' two times.

5.Click the Display Options separator

If the number in the Number-of-Vertices box is zero, or a number is not in the box

6.Click the 'Import Model from SOLIDWORKS' button again, and wait until the button releases.

When the Number-of-Vertices is not zero...

7.Click the Colour button to edit the colour of the SOLIDWORKS solid in the graphic-area.
8.Click OK.

tog_minusProcedure 2: Import a SOLIDWORKS Sub-Assembly onto one CAD-Line

If the sub-assembly has many parts and features that are not necessary - for example washers, screws... - then in SOLIDWORKS, create a new Configuration.

In the new SOLIDWORKS configuration, suppress parts and features in parts that you do not need to see in the MechDesigner model. Also, replace fillet with chamfer features from parts.


1.Make active the configuration in which you have suppressed parts and features.
2.Add a Plane and Coordinate System - see Procedure 1, above.


See Procedure 1 above

You may need to press the 'Import Model from SOLIDWORKS' button two times.

If you have already imported a SOLIDWORKS model, then you will need to delete the STL from the model path.

Note: The Mass-Properties [see Mass-Props tab] become the Mass-Properties of the Sub-Assembly, taking the different materials and shapes into account.

tog_minusProcedure 3: Import different SOLIDWORKS Parts onto different CAD-Lines

In SOLIDWORKS, it is often best to mate the Parts into a 'working' assembly before you import the different Part, if they are not already in an assembly. This will help you make sure the Coordinate Systems are on the Same Plane.

Import each Part form SOLIDWORKS onto a different CAD-Line. Each CAD-Line may be in the same or in different MechDesigner Parts.

CAD-Lines in one Part:


At the top level of the assembly, add a Plane. We call this the Master Reference Plane.
Edit each Part you will import from SOLIDWORKS to add a Plane that is coplanar with the Master Reference Plane
Add a sketch to the Planes in each Part, and then a Coordinate System.
Make sure each Coordinate System is coincident.

In MechDesigner:

Add an equal number of CAD-Lines to the Part as the number of parts you will import from SOLIDWORKS
Make the start-Point of each CAD-Line coincident
Make the CAD-Lines co-linear
Rename each CAD-Line to the same as each SOLIDWORKS Part.

CAD-Lines in different Parts:


If necessary, add a Master Reference Plane at the top level of the assembly.
Add a Plane, that is coplanar with the Master Reference Plane, to each Part you will import from SOLIDWORKS
Add a sketch to the Plane in each Part and then a Coordinate System.
Make sure each sketch and Coordinate System aligns with the CAD-Line in the respective Parts.

In MechDesigner:

Typically, you will import the SOLIDWORKS Parts onto one or more CAD-Lines along the center of each Added-Part.
If necessary, if you also want to add more than one SW parts to a MD Part, add more CAD-Lines to the MD Part. As above, make the CAD-Lines co-linear and their start-Points coincident.
Rename each CAD-Line to the same as each SOLIDWORKS Part.

Then follow MechDesigner Procedure 1 - see above.

Do Procedure 1 again and again, with all the CAD-Lines and Parts you want to import to MechDesigner from an assembly in SOLIDWORKS®.

tog_minusTrouble-shooting: Active Document does not show in MechDesigner

Occasionally a Part, and more often an Assembly, does not import or show in MechDesigner:


Make sure there are not any:

small/tiny, but real, gaps between parts
small parts with complex details - for example, a set-screw.

In the MechDesigner CAD-Line dialog-box and SOLIDWORKS tab

1.Change the File-Quality to Custom, and edit the Linear and Angular Deviation parameters.

Experiment with the Linear and Angular Deviation parameters to import a Solid with 'fine' details, or with 'coarse' details.

tog_minusUsing the STL File Import separator in the CAD-Line | Solids tab.

STL File Import separator - If you have SOLIDWORKS, you do NOT need to use this control.

Unfortunately, we do not recognize Planes and Coordinate Systems in STL Parts.

Thus, you must move the Part in your CAD to align with the CAD-Line.

Edit the model in your CAD Program:

1.Move a Point/Vertex to (0,0,0) of the Model Coordinates.. It will locate at the Origin of the CAD-Line.
2.Move the model to make a Line/Edge align with the +Xaxis. It will become aligned with the CAD-Line.
3.Make the model so that a Line/Edge aligns with the +Y-axis. It will align with the +Y-axis of the CAD-Line.

Save the model as a binary STL file-type. The units of the model should be meters.

To Import the STL File:

1.Edit a CAD-Line, and click the SolidWorks tab
2.Click the STL tab
3.Click the Browse...button: .to find the STL file you would like to import.
4.Click the Convert STL to MD Solids button: to import the STL file.

Tutorial and Reference Help Files for MechDesigner and MotionDesigner 13.2 + © Machine, Mechanism, Motion and Cam Design Software by PSMotion Ltd