Working with Imported CAD


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Designing from scratch in Onshape isn't the only way to build and refine your CAD models. If you have existing CAD data in another system, you can import that data into Onshape and continue designing here.

Onshape accepts data from many other systems, the most popular and well-translated being Parasolid files. For more information on file types accepted and how to import your data into Onshape, see Supported File Formats and Importing Files.

This topic explains how to proceed and what tools are available after you've imported your existing CAD data into Onshape.

Onshape tools

Due to system differences, data imported into Onshape may translate in with faults, or no parametric history, or as a series of surfaces or parts instead of a solid or cohesive body. While you have some options for how data will be handled upon import, there remain some things beyond control. However, Onshape has tools that will help you move forward with your imported data and work with it to continue designing, sharing, and releasing designs.

The tools provided to help you work with imported CAD data and covered in this topic include:

  • Mesh - Change units for meshes post-import into Onshape
  • Repair imported models - Identify holes and disconnects in imported models that may require repair.
  • Create composite parts - Create composite parts out of parts or surfaces fractured during the import process.
  • Edit imported parts with direct edit tools - Including modify fillet, delete face, move face, and replace face
  • Update imported parts - Update imported parts from within Onshape when the source file from another system is updated.
  • Replacing one reference with multiple references - When parts are linked within Onshape, you can replace a referenced part with multiple parts, if desired.

Mesh

Onshape enables you to import three faceted file formats: STL, OBJ and Parasolid Mesh for visualization and referencing. Mesh points are able to be used as vertices for creating planes.

A mesh is imported into Onshape Part Studio, and shown in the Parts lists under Meshes (below Surfaces).

You can view and reference meshes, but you can not edit them.

You can change the mesh units during the import process and from the units dropdown within the tab menu, shown in the second image below:

During import, above

Within the imported tab, above

What you can do

Once a mesh is imported into an Onshape Part Studio, you have the ability to:

  • Create a three point plane using mesh points

  • Measure the surface area, distances to and from mesh points, and mass properties for solid meshes

  • Project mesh points in a sketch (via the Use tool)

  • Create Mate connectors at mesh points

  • Reference a mesh point for ‘Up to vertex’ operations (as in Extrude)

Meshes are not supported in Assemblies or Drawings.

Repairing imported models

Onshape provides a tool for identifying holes and disconnects in imported models that may require repair: Highlight boundary edges.

Highlight boundary edges can be found as a menu option in the View tools cube: Highlight boundary edges.

When Highlight boundary edges is selected, boundary (or laminar) edges are displayed in solid red lines (for visible edges) and dashed red lines (for hidden edges).

To repair these surfaces, you can use any number or combination of tools in Onshape, for example:

  • Enclose - Select surfaces, faces, and parts that enclose a region to create a new part.

  • Fill - Create a surface bounded by a closed set of curves or edges.

  • Move boundary - Move boundary edges of a surface in order to extend or trim it.

  • Bridging curve - Create a curve connecting any two points or vertices.

  • Composite curve - Create curves from selected edges, sketch entities and other curves.

Creating composite parts

When parts or surfaces are fractured upon import, or when you want separate bodies to be treated as a cohesive unit, create either a closed or open composite part (one which consumes the entities, or does not, respectively).

For example, if your design is fractured upon import, as in this example below where one section of the design is rendered as multiple surfaces, you can select the fractured entities and combine them to form a composite part:

The selected surface, "object_1(13)," is cross-highlighted in the model - but suppose you want all the surfaces to be one part. You can select them and create a composite part, shown below:

The part, after the feature is accepted:

Editing imported parts with direct editing tools

Imported geometry does not carry with it the parametric history so there may be times when you need to use Onshape's direct editing tools to continue modeling an imported design.

For example, after you import a part, the holes might be in the wrong places. You can use the direct editing tools to remove the original holes and then make new holes in the proper locations on the model.

Another example is fixing imported geometry when a face is missing or has an error, or you have to delete a face and recreate it. In the example below, the knob on the top of the cap needs to be reshaped, so the Delete face tool is used:

The imported cap with knob, above

The selected face to remove, above

The resulting cap with new face, above

Updating imported parts

Parts imported into Onshape can be updated if the source part has changed. The first thing to understand is where Onshape stores that information. Depending on where you initiated the import in Onshape, the part will be in one of two places:

  • Import from the Documents page and the part is inserted into a new document bearing the same name as the imported file.
  • Import from within an existing document and the part is inserted into a Part Studio bearing the same name as the imported file.

In both cases, you will find a folder by the name of CAD Imports and within that folder, a tab with the same name as the imported file. Also in each case, you will find a Part Studio with the same name as the imported file. You can change the names of the folder as well as the tabs.

After a part is imported, you can update it should the part change in the source file.

To update a previously imported part:

  1. Export the part once more from the other CAD system. (Presumably this part has been changed since the first time it was exported.)
  2. In the document into which the exported part was previously imported, you can proceed in a either of two ways:
    1. Open the Part Studio that holds the part, right-click the Import entry in the Features list and select Update.

      Before Import Update

      Feature Menu with Import's dropdown menu and Update highlighted

      Select the export file and click Open. The Import feature updates to the updated part.

      Updated Import

    2. The other option for updating an import feature is to click the folder titled CAD import and select the tab of the imported file. Click Update (shown below), select the export file and click Open. The new file name is displayed and the part is updated in the Part Studio.

      Pre-Update Importa

      The new file name is displayed and the part is updated in the Part Studio.

      If a document has not been upgraded after Onshape release 1.93, then this Update button will not upgrade the imported feature but will instead make a new Part Studio containing the new/upgraded part. If the document has been upgraded since Onshape release 1.93, when the Update button is clicked, the imported blob is updated with the new file and the updated geometry propagates to the imported feature.

      Post-Update Import

In both cases, the Part Studio containing the Import feature is updated.

What is updated

When a part is updated, all features and changes made to the part in the source system are updated in the target Part Studio. If the part has been modified in the target Part Studio, by applying features to it, those features are reapplied to the updated part where possible.

For example, if a fillet has been applied to the part in the target Part Studio, that fillet is reapplied to the updated part where possible. There may be modeling changes made to the source part that result in applied features in the target Part Studio from regenerating successfully. These features will be shown in an error state in the Features list.

Deleting imported files

When deleting imported files, you will see a warning about which Part Studios the deletion will impact:

Delete File Tab

Replace multiple references with one reference

Sometimes when you import a project into Onshape, commonly used components may become duplicated. Since duplication of components is an undesirable situation, in Onshape you can instead use multiple references to the one component.

For organizational purposes, it's best to move the common component to its own document, so all users can find it easily without disturbing projects in process. To move a component out of one document and into another:

  1. Select the name of the component in the Part Studio's Parts list.
  2. Right-click and select Export.
  3. On the Documents page, click Create and then Import.
  4. Import the file you just exported, which will create a new document.
  5. In the original document, locate the part in its original Part Studio.
  6. Delete the part from the Part Studio.

    Note that in this document, all references to that Part (in assemblies) will 'break' and appear red.

  7. In each assembly that references that part, select each reference to the part in the Instances list, right-click and select Replace parts.
  8. In the Replace part dialog, navigate to the Created by me document section, and select the new source document containing the common component.
  9. Now the component will be inserted where it was referenced in the assembly, but with a link icon next to it. The link icon indicates that the instance is referenced from another document.

The advantage to this workflow is that you now have one component instanced many times. If you want to make a change to the component, do it in the source document and then you can decide if and when to update the instances referenced in other documents. This saves you the trouble of reinserting and mating multiple components unnecessarily, as well as aid you in keeping components up to date easily.

For a more in-depth example, see this Onshape Tech Tip.