IGES and STP file modification

[TomBW]

Does anyone know how to modify an IGES or a STP file while in Solidworks? I am not able to access to the sketch menu from an IGES or STP file that I have downloaded.

Thanks,
Tom

[Elgin Clock]

IGES or STEP files come into Solidworks as one entity (or seperate parts consisting of one entity each if it is an assembly).

You will not be able to access the part's "tree" structure like you can if you started it from scratch in Solidworks, because it only comes in as one entity.

What kind of part are you looking to modify?
What specificially are you trying to do with that part?

For instance, if you are trying to remove a hub from a sprocket, just start a sketch on the top of the hub's surface, convert the outer circle of the hub with the "convert entities" command and "cut extrude" through the geometry to remove it.

To add geometry, do the same but use the extrude command.


If you can provide a link to the (IGES or STP) part file in question, and let me know what you want to do with it, I can take a look at it and see what the best approach would be.

[Andy A.]

A little background on IGES and STP-

These formats were made to be easily exchanged between solid body modeling software. As such a STP or IGES file can be opened by virtually any CAD package.

The downside is that the model is stripped of any program specific information. So sketches, feature information, physical properties and so on are gone. It becomes a single solid body, and depending on the geometry, a simplified one at that.

It's kind of like saving a word processor file as a .txt instead of .doc. You know that anyone anywhere will be able to open it, but it's not going to have any formatting when they do. It's a trade off you make solely for interoperability now and in the future. Unless you plan on working across platforms (like inventor and solidworks), STP and IGES probably won't do you much good.

-Local

[mplanchard]

Tom

If you have the SolidWorks Education Edition or your mentor has a SolidWorks Commercial Edition you can utilize the Add In called Feature Works to make non parametric features from IGES/STEP/SAT into recognized ones.

Also from within SolidWorks, you can select on a face from imported geoemtry, create a new sketch and extract geometry in a Sketch with the Convert Entities tool. This technique is usually the most helpful because you really dont want to spend a great deal of time converting all imported parts in an assembly if you just want to add a few holes to a mounting plate.

Marie