Welcome to 3DCADForums

Join our CAD community forums where over 25,000 users interact to solve day to day problems and share ideas. We encourage you to visit, invite you to participate and look forward to your input and opinions. Acrobat 3D, AutoCAD, Catia, Inventor, IronCAD, Creo, Pro/ENGINEER, Solid Edge, SolidWorks, and others.

Register Log in

The meaning of different gear icons

araminaran

New member
Hello all
in design tree, when we create or insert a body, we will have an icon which always has a specified shape expressing something like for example the positive sign indicates a link with another part. So what is the meaning of attached icon, For example the green and blue gears? I appreciate if anybody has a brief description of each symbols of icons.
Thank you all
 

Attachments

Last edited:

MrCATIA

Super Moderator
In CATIA V5, the different icons are clues about your CATIA files. Most of the icons indicate the status of that feature; some icons indicate an error. Understanding the different icons are very helpful to troubleshoot a file. The icons and their descriptions are described in the CATIA online documentation.

In a CATPart file, the following icons can be found in front of Bodies:

Single green gear this represents the primary Body of a part.

Green and blue gear this represents a secondary Body of a part. A small yellow "+" sign indicates a positive body (as seen in the attached image above), and a "-" sign indicates a negative body. This body can be deleted; a primary body cannot be deleted.

Yellow gear this indicates the body contains hybrid features (solid and surface) but the options are set for non-hybrid mode

Silver gear this indicates the body is non-hybrid (contains solids only) but the options are set for hybrid mode
 
Last edited:

MrCATIA

Super Moderator
some follow-up comments about bodies in general:

- Bodies with green gear icons are good. This indicates the part matches your CATIA settings, and the part will remain in that mode as new features are added.

- Both Hybrid and Non-Hybrid modes are OK. It's just depends on which mode you're most familiar with. Sometimes your company may require everyone use one method only. Problems occur when you try to mix the two modes.

- A Non-Hybrid part can be converted into Hybrid.

- A Hybrid part cannot be converted into Non-Hybrid

- CATPart files containing multiple bodies are usually not required. A good example of a multi-body part is one that is made of different materials, such as a metal insert with a rubber overcoating.

- Multiple bodies are required for Boolean Operations, which are sometimes used for complex parts.
 
Last edited:

MrCATIA

Super Moderator
another comment:

- Be careful with "-" (negative) bodies. They behave in reverse: additive features will remove material, and subtractive features will add material. Very confusing to work with.
 

araminaran

New member
thank you dear sir. your helps are greatly helpful. I enjoyed your comments:) . But I think there is a problem with your last comment. It is in contrast with what you wrote previously. you said upper:
A small yellow "+" sign indicates a positive body (as seen in the attached image above), and a "-" sign indicates a negative body. This body can be deleted; a primary body cannot be deleted.
but later you added:
Be careful with "-" (negative) bodies. They behave in reverse: additive features will remove material, and subtractive features will add material. Very confusing to work with.
I'm a little confused. for your last comment, I think the opposite is the case. isn't it?
 

MrCATIA

Super Moderator
It depends on the Current Work Object, and if you're using Boolean Operations.

My last comment is true, if the Current Work Object is the negative body. Features in that body behave in reverse.

If the Current Work Object is such that the negative body appears as an Assemble Operation to other bodies, then the features behave normally.
 

Sponsors

Forum Sponsors

X
Top