Pourquoi mon modèle xShape est-il latéral dans SOLIDWORKS ?

Article by TriMech Solutions, LLC updated February 23, 2023


SOLIDWORKS and xShape (3D Sculptor) are two of the most popular modeling tools available within the 3DEXPERIENCE ecosystem. These two applications have a lot in common, but it is important to be aware of their differences. One key difference between SOLIDWORKS and xShape is the orientation of their modeling environments. If you’ve ever wondered why your xShape model is sideways when brought into SOLIDWORKS (or vice versa), keep reading to learn why.

Y-up and Z-up Orientation

The reason parts sometimes import “sideways” when switching between SOLIDWORKS and xShape is because they have different modeling environment orientations. SOLIDWORKS uses Y-up Views, whereas xShape (and all other xApps) use Z-up Views. The “up” direction specifies what the “Top” standard view is, and all other standard views (Front, Right, etc.) are based upon that. The “up” direction also specifies the orientation of the 3 starting primary planes. When a model designed in one application is imported into the other, the model will not be oriented properly if the modeling environments’ orientations did not match.

Below is an assembly that was modeled entirely in SOLIDWORKS. We can see that the Top Plane faces upwards in the direction of the Y axis of the triad in the lower left corner of the screen.

Assembly modelled in SOLIDWORKS

In the xApps such as xShape, things look a little different. Below, you can see a model that was designed using only xDesign and xShape. The chair icon in the upper right corner of the environment helps us understand which way is Front, Top, Right, etc., and shows the XYZ triad as well. However, here you will notice that the Z axis is pointing up, and aligns with the Top view.

xShape Monitor stand

Importing xShape model into SOLIDWORKS

Let’s take a look at the Base Cover from the image above. As you can see below, this model was made in xShape, and is oriented properly inside the xShape “Z-Up” environment.


When inserted into SOLIDWORKS, the model appears sideways. This is because it is still using the Z axis to define its “Up” orientation.

Le modèle semble latéral

Solution #1: Rotate using Move/Copy Body

A simple way to remedy this issue immediately is to use the Move/Copy Bodies command and apply -90-degree rotations about both the X and Y axes, as shown below:

Solution #2: Change SOLIDWORKS from Y-Up to Z-Up

Another way to remedy this issue is to make SOLIDWORKS use Z-Up orientations. To do this, select the View Orientation cube from the Heads-up Display toolbar, then click More Options. (Or simply press the Spacebar on your keyboard). From the View Orientation window, select the Up Axis Flyout, and select “Apply Z-up views”. A message will appear: “Switching to Z-up views will change the orientation of any standard orthogonal, named, and child views in drawings of this model. Do you want to make this change?” This message is warning you that changes made to this model’s orientation will propagate into any related Drawing files. Click Yes to continue.

Changing the orientation of a part

After applying Z-up views, your model will align with the triad in the lower left corner, and you will find that your standard views are correct. However, the Primary Planes (Front, Top, and Right Planes) are not automatically renamed, as seen below.

Planes shown in xShape

It is recommended at this point to Rename the Planes to reflect their orientation relative to Z-up. The Planes should be as follows:

  • Top Plane faces “upwards”, normal to the Z axis
  • Front Plane is normal to the X axis
  • Right Plane is normal to the Y axis

See the Planes I renamed below.

Renaming planes

Making a Z-up Template

If you are working between SOLIDWORKS and the 3DEXPERIENCE xApps often, it may be worth it to create a Z-up SOLIDWORKS Part template. To do so, start a New Part, and while it is blank, Apply Z-up views and rename the primary planes using the steps above. Then, go to File > Save As (Click “Save to This PC” if a 3DEXPERIENCE pop-up window appears). Change the File Type to Part Template (.prtdot) and save.

Then, you can use this template whenever inserting an xShape file into SOLIDWORKS and it will automatically be oriented properly. Additionally, you can use this template when creating new Parts in SOLIDWORKS. That way, if you need to insert a SOLIDWORKS Part into an xApp like xShape, you will already have the correct Z-up orientation upon import.

Save a new part in xShape

An assembly template can be made following similar steps: Start a New Assembly, and while it is blank, Apply Z-up views and rename the primary planes using the steps above. Then, go to File > Save As (Click “Save to This PC” if a 3DEXPERIENCE pop-up window appears). Change the File Type to Assembly Template (.asmdot) and save.

To learn more about using SOLIDWORKS with xShape through 3DEXPERIENCE, check out this On-Demand Webinar: Little known tools you already own on the 3DEXPEIRENCE platform using 3D Sculptor with SOLIDWORKS.

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TriMech Solutions, LLC

TriMech fournit à des milliers d'équipes d'ingénieurs des solutions de conception 3D et de prototypage rapide qui travaillent main dans la main, de l'esquisse à la fabrication. Javelin est devenue une filiale de TriMech Solutions LLC en 2021.