Simulate Idea

[rubenvillarreal]

Hello,

Simulate lets you perform analysis using symmetries (either cyclic or mirror). The problem is that in order to use symmetries, you have to create the part or assembly using Creo.

It should be cool if simulate allows you to cut or remove material from a non-creo model. In that way, you can simulate a turbine modeled in Catia or Solidworks using symmetries, avoiding that your computer fries with each blade.

That's all.

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[mlindqvist]

You can easily cut a model created in non-Creo CAD system, this works fine. If it's a surface model (i.e. iges), you might need to patch up your surface so that it becomes "water-tight", then solidify it. With STEP, if exported as a solid, you can add/remove geometry, add rounds/holes etc.  as usual. With the "feature recognition tool" you can "parameterize" rounds, chamfers, holes etc. so that you get features in the model tree, with parametric control.... I don't have experience from other tools, but in my view Creo is a great tool for manipulating imported geometry. Provided you have a Creo Parametric license of course... Otherwise you can just ask the creator/owner of the orignial CAD-file to cut it for you. 

[rubenvillarreal]

Now I realize that I can (as an assembly part).

Can you explain me how this work: "With the "feature recognition tool" you can "parameterize" rounds, chamfers, holes etc."

Thank you.

[mlindqvist]

The feature recognition tool is under the "Get data"-menu, see picture below. For example, if you want to turn a fillet into a regular round-feature that you want to modify or delete, click "Search fillet", click on the fillet, and then "OK". Your model will appear identical, but in the model tree, you will see two new features. First a "remove"-feature that removes the fillet. Then you will see a new "round" that reproduces the previous fillet with a new parametric "Creo-round".

I mostly use it to delete fillets,chamfers etc. from an imported model. In such cases I first use the "feature recognition tool" and then I simply delete the round/chamfer etc. and keep only the "remove"-feature.

I hope it helps...

B.R. Mats L

[rubenvillarreal]

Excellent information.

Thank you!

[unickque]

I don't think this Feature Recognition is part of standard Creo/Parametric.

In any case, I do not have it in my Creo2 here at work, which has the following options:

347	Freestyle_Design_Extension	ModelCHECK
4DNavigator	HARNESS-MFG	NOTEBOOK
AE	INTERFACE	Options_Modeler_Basic
ASSEMBLY	INTF-CADDS5	PHOTORENDER
Behavioral_Modeler	INTF-CADDS5	PIPING
CABLING	INTF_for_STEP	PLOT
CDT	Import_Data_Doctor	PROCESS_ASM
COMPOSITE	Interactive_Surface_Design	REPORT
Collaboration	Intralink_8_0	SCAN_TOOLS
DATA_for_PDGS	LEGACY	SHEETMTL-DES
DETAIL	LIBRARYACCESS	SURFACE
Design_Animation	Layout_3D_Integration	Truly_Heterogenous_Assembly
ECAD	Manikin	WELDING
FEATURE	Mechanism_Design	Web.Link
Flexible_Modeling	Mechanism_Dynamics	Web.Publish

[mlindqvist]

As I understand it, FRT does not require any additional license, bút you need to set a config option,

From PTC support:

Resolution

For Creo Parametric 1.0, 2.0 and 3.0 To use Feature Recognition Tool (FRT), no additional license features are required FRT can be used with any base Creo License packs To enable Feature Recognition Tool (FRT), add configuration option frt_enabled yes and then launch Creo Parametric Note that setting this option in session will not make the FRT menu available For the menu to be accessible, a model must be open with at least one import feature containing geometry from a Boundary Representation model (IGES, STEP, etc., but not facetted surfaces) Otherwise the menu is available, but grayed out The FRT commands will be under Model > Get Data > Feature Recognition

https://support.ptc.com/appserver/cs/view/solution.jsp?n=CS28594

[JonathanHodgson]

Ooh - does this mean it's available in Creo 2?  I'd been under the impression it was a Creo 3 enhancement.

[unickque]

Yes it is, just tried it. Thanks for explaining Mads

It even works okay, though it seems to have some quirks. Selecting a hole surface did not work, selecting an edge worked okay. (On a simple hole with straight surfaces on both ends, in what is a small but quite complex STEP file of a machined casted part).

[mlindqvist]

Yes, it's in Creo 2. I use it all the time when I deal with imported geometry. Even if it is native Creo geometry, it is sometimes convenient to export a step-file that I then re-import to work on that instead of the original Creo file. When I prepare a CAD-model for analysis, it is sometimes a lot of work to change something if the model tree lights up like a christmas tree when you try to change something. With a step export-import, you eliminate all dependencies. 

[mlindqvist]

No, in this case I would typically suppress rounds/holes etc. in the original Creo file. Good modeling practice means keeping rounds chamfers etc late in the model tree, if this is applied then it is usually easy to get rid of such features. If you have a lot of references that would be affected by suppressing for example a hole,  then I might use the export-import technique, and remove the hole in the imported "dead" geometry. 

[unickque]

You work for the only company that I know of which has a Reverse Engineering Department

[rubenvillarreal]

Yes! Uniform thickness and I shell them, this was only an exaggerate mesh about the problem of removing material. I am still unable to use the FRT, it just doesn't appear. Can you upload the model of your picture?