CATIA V5: Creating Drawings from CGRs

March 1, 2021 Scott Henderson

In this post, we’ll look at how to create drawing views from lightweight CATIA files.

See Gee Are What?

The CATIA Graphics Representation (CGR from here on out) is a lightweight file format for CATIA. In general, the outside “skin” of a CATPart is tessellated and saved, leaving only the shape data behind. This is great for visualization – file sizes are way smaller and it’s easy to work with big assemblies without a huge performance hit. Of course, there are some trade-offs: Namely, all the part feature data is gone. Anything that needs “real” geometry is not going to be happy with a CGR.


Problems in Lightweight Land

Now and then, for whatever reason, there is no CATPart file to work with and you’re stuck with a CGR. Assembly constraints generally won’t work. Changing the shape data isn’t completely impossible, but for all intents and purposes, it’s not something that can be done. Drawings… generally do not want to cooperate with CGRs. (At least, not without a little push.)

In the image below, I’ve got a part that has been saved as a CGR. CGRs can’t be opened directly, so I’ve got this one in an assembly, where they’re typically encountered.

Hovering over various surfaces of this part causes a lot of triangles to be visible. This is one of the key giveaways that we’re working with CGR data.

Attempting to expand the CGR tree does nothing. Check out the icon for the CGR. It doesn’t have a sheet of paper behind it like part and assembly do.

Now, heading to the Drafting workbench and creating an automatic drawing with all views yields the error below:

While the message gives some advice, none if it is actually the solution to this issue. Okaying that box does not leave much of anything to work with. There’s an empty sheet and little else.


View Modes

To get a drawing view from a CGR, head to Tools > Options > Mechanical Design > Drafting> View and set the “View generation mode” to “CGR.”


This will allow CATIA to generate drawing views from CGRs. No more errors and now there are views to work with. Great! That is, with a few caveats. 

Views from CGRs aren’t nearly as flexible as Exact views from parts. Most of the dress-up options are not available, dimensions may be inaccurate, and some irregularities in the geometry may appear.

A Hybrid Approach

Sometimes you’ll find large assemblies have been built with a combination of CGRs and CATParts. Maybe most of the parts have been simplified to CGRs to help keep the file size down and keep the big assembly manageable. A few files might still be CATParts that contain important wireframe data or maybe even Functional Tolerancing & Annotation Data.

These will be a little bit easier to work with.

In the pictures above and below, I’ve got the same assembly as before, but this time it has a Reference Data part that contains a wireframe point and a surface.

Using the default CATIA settings (Exact view mode), I’m able to generate a drawing. However, there’s not much to display – only the exact Fill.1 surface shows up. The good news, though, is that there are drawing views to work with.

Instead of digging through Tools > Options, right-click the drawing view(s), head to the Views tab, and adjust the View Generation Mode.