from an Asm need to create Datum curves from an Xsec

[texaspete]

Hi gang, I think in some help, I have an assembly of parts the parts are surface data (.prt files) and solid data (.prt files). I search the website - looked for "Xsec" and nothing was found. I found one of my old posted from last year - but didn't have an answer. This is my goal. I need datum curves from a Xsec (Section c-c to be specific). These datum curves? would it be located or created in another file. I need to know the step to create 2d datum curves which will be used in another file.
thanks Texaspete

 

[robertib]

It seems to me that you are asking one of 3 questions.
how to create a 2d datum curve?

how to create an offset Xsec?

where is the detail of the Xsec located?

More details of what you are looking for would be appreciated.

 

[texaspete]

Hi Robertib, Sorry for the lack of info. THe application is a new tail lamp design. The file is an assembly, the part files data is a mix of Surface parts and solids parts. The section is thought y=770mm about the middle of the assembly. This is the application, I am working on a new tail lamp design. I have created a Xsec using the View Manager. In the view manger the section is named “Section_A-A”. I can see the yellow curves but I can use them but to create a view in ProDetail. The goal is this the cross-section (Section_A-A) is in car position and that section needs to be IGES, or Step out in car position and then be translated into CATIA V5 in car position. Just an FYi, I can't used the "Used edge" located in sketcher. The section is planar if this helps.
Thanks Texaspete

 

[Guest0527211403]

hi texaspete

There is a curve from section tool that can be found under Insert-->Model Datum-->Curve, and then select Use Xsec.

The curve must be a feature in the same part or assembly where you have made the cross section.

You can make a part from this curve to export to catia as well:

-Use Insert-->Component-->Create and assemble the new part in the default location.
-Right Click on the part and select Activate.
-Select Insert-->Model Datum-->Curve and then select Copy
-Pick the curve you just made

You can now open the new part on its own and it should only contain the curves from the cross section, located in the correct position wrt the vehicle which you can export.

 

[texaspete]

Thanks Justkeepgivener That WORKS WONDERFUL. I'm tipping my beer glass and hat to you.
Texaspete

 

[Guest0527211403]

careful, don't spill any beer.. and don't keep beer in your hat. i tried that once with disastrous consequences.

 

[ian99rt]

I'm guessing this is the same question i have. I have a splined shaft that I need to make a cut of the same splined cross section. Is this the same process I want to take?

 

[Guest0527211403]

Not necessarily, since this method will create a number of dependencies on the assembly to which everything is modeled. So if you try to load up the part the splined shaft fits into on its own, you will get a failure (since the assembly would need to be loaded up).

You might want to copy in the curves using a copy geometry feature Insert-->Shared Data-->Copy Geom from other model. This lets copy surfaces and/or curves without an assembly dependency.