Pro/Welding

[bartL]

Hello,
I know this isn't the right place for this question, but there's no Pro/E forum in the CAD section. BTW Why not???
I'm trying to create some welds in a simple assembly with the pro/welding mode (licence). Now I would like to create a STEP file so I can use it in another program but I can't make the welds solid, it stays a surface between the welded parts. Does anybody here works with pro/welding and know how to do this?

Thanks,
Bart

[JonasC]

Hej Bart,

If you have a legit copy of ProE and especially a maintenance agreement you can find this info at ptc knowledgebase here:
https://www.ptc.com/appserver/cs/vie...?n=/123671.htm
If not, let me know and I'll give you the headlights.

BR, J

[bartL]

Jonas,
I don't have permission to login on the PTC site
So I wpuld be very thankfull if you can give me te headlines. I'm especially looking for some method to create realistic welds (if that's possible) which I can use for strength calculations in another program.
Thanks for the reply in the corner round thread.


Thanks in advance,
Bart

[JonasC]

ok, for this time I will cut&paste from ptc.com, but since I doubt they appreciate that it's this time only.

=======================================================

Description
-----------------
Possibility to show weld features as solids because they look like as surface features.

Alternate Technique
-----------------
In assembly mode create a new part and create a swept protrusion for example referencing edges from both connected parts.

Resolution
-----------------
Weld features are surface features and cannot be shown as solid features in generally.
Exception:
For cross section drawing views there is the possibility to set drawing setup option "weld_solid_xsec yes".

Further information can be found in TPI 102781 for the config.pro option hlr_for_quilts and TAN 111852 for the drawing setup option show_quilts_in_total_xsecs.

=======================================================

Which basically means, you can't do it in any simple way.
What you can do is simply reference the resulting curves and (re)model the weld as solids.

best of luck, Jonas

[bartL]

Jonas,
Thanks for this information.
Do you have any experience with one of these solutions?
I've tried to create parts in assembly mode before (which I think is the best way to create realistic welds) but it always says that I can't use references from parts in the assembly. If I can use references from other parts it would be much easier to create a sweep trough the model.

Thanks,
Bart

[JonasC]

Originally Posted by bartL Jonas, If I can use references from other parts it would be much easier to create a sweep trough the model.

Sure would!
ProE is set, default I think, to minimize external dependencies. I guess this is due to the fact that too many references back and forth might make your head spin. However, it's obvioulsy a very strong tool.

When in an assembly, go to 'Tools' / 'Assembly Setting' / 'Reference control'
Set it too 'All'.
Besides the option to reference other parts you now also have the option to merger several parts together into one single part. This can be done in many ways, but I think you want to look in the 'Insert' menu when in assembly mode.
First of all put an empty part into your assembly. Rightclick on it in the feature tree, and select activate. Now you can copy other parts into this from the 'Insert' menu. Pick 'Shared data' at the bottom and then 'Merge'. Other options are there as well so have a look at them.

good luck, J

[bartL]

Jonas,
Thanks again for this info.
Where are you using this merge function for? I've never used it since I'm working with pro/e daily for work for 1,5 year now.
Are you common with pro/e models used for strength calculations (like mechanica or another program)? I'm trying it for the first time now and it works pretty good. But now I'm trying to get a realistic fatigue lifetime calculation for welding assemblies and that seems to be very hard since you have to take account with lots of values like material properties and changes because of the temperature influence. Beside that a realistic model is very important too, and even that seems to be quit a job to get it correct.

Thanks,
Bart

[JonasC]

Bart,
np, glad to help.
About the merge function, it can be used for various tasks. What comes to mind as I'm writing this is to simplify an assembly into 1 single part, for analysis or similar. In some design tasks you can benefit from doing the target part as a merged part. I use it pretty often but I can't really tell for what becuase it's different from time to time.
It's opposite is the 'cut out' operation which is basically a boolean operation subtracting one(or several) piece(s) from another.

About the strength calculation, ye, I've worked some with Mechanica. Wouldn't call myself an expert maybe more of a somewhat advanced user. Also been playing around some with Abaqus and Ansys.
Fatique calculations have I never done though. There seem to be so many pitfalls in that area so I leave that to the ppl doing calculations for a living

Been using ProE (almost) daily for 9 years now btw....

/jonas

[bartL]

Aha,
It seems we can't use that merge function in the company I'm working for because we are always working with the complete set of production drawings in the factory. In other words every assembly stays an assembly with the 'child' parts attached to it so everyone who has the permission can see how the assembly is build. Beside that the whole structure of the machine is in our PLM system and is linked with some other calculation programs, so it is neccesary that every single part is in that structure. The only thing we could use it for is converting a welding assembly in a casting part. That makes an assembly become a part. Mostly when I do that I simply save a copy as an IGES and open it as a part, then save again.

I've never worked with mechanica but I've heard it's quit a strong application. I'm working with ANSYS which is the best FEM analysis sofware in my opinion, but as I've said before it's a pain to get a good welding assembly in ansys, since I want a realistic weld which is even a bit in both parts (the notch).

Hopefully I'll find a good solution to create those kind of parts in an easier way.

Thanks,
Bart