Cannot make the "PTC_MATERIAL_NAME" parameter flexible????

Forum|Forum|7 years ago
January 24, 2019
9 replies
4941 views

I'm adding flexibility to my library fasteners to get them to fill out the repeat regions of the parts lists the way I want, yet when I went to make the parameter "PTC_MATERIAL_NAME" flexible it was not on the list. If I can't make that flexible it REALLY throws a monkey wrench into my plans.

Does anyone know if there's a Pro/WORKAROUND for this? Or am I simply stuck using the Pro/FANITY module (again...)?

Grazie!

General

Best answer by pausob

Well, before posting, I tried the technique I suggested and it worked on my system. But I'm still using Creo 2.0. Maybe this was "fixed" in later version.

And if "flexed" bolts work for your company - that's great! Do you guys use Windchill to report the BOM? Because I'd be curious as to how you manage to report the different bolt instances.

P

pausob

19-Tanzanite

I'm not sure using flexibility for fasteners is a good idea - but hey - to each his own.

The only Pro/Workaround I can think of is to put into your flexible model a string-type parameter, let's call it "MY_MATERIAL", and a relation:

PTC_MATERIAL_NAME=MY_MATERIAL

However, you lose the key feature of the PTC_MATERIAL_NAME parameter: the drop-down list from which you select one of the multiple materials that are saved in the part. Without this list, the end-user of your model will not know what to type into the MY_MATERIAL's new value column when they bring it into their assembly.

Patriot_1776

Author

22-Sapphire II

Actually making fasteners flexible works great. In our case, sometimes we use MIL-SPEC fasteners, in some cases McMaster-Carr fasteners. Depends on the application. No sense in using expensive certified fasteners for non-critical assemblies. Using flexibility allows the user to use the same fastener model carefully created to the appropriate specification (instead of your typical vendor import garbage), yet be able to easily modify what shows up in the parts lists (i.e. Vendor, Vendor P/N, MS part number, MIL-SPEC, material (text-string not driven by or driving PTC_MATERIAL_NAME), etc.). Also, in our particular industry, we sometimes have to use very exotic fastener materials to deal with the extremely harsh environment some of these assemblies are designed for. In addition, I have made a closed-and-ground compression spring library model that, with the flexibility I've built in (OD, wire dia, number of turns, free length, material, and the others I've listed above), this one non-family-table model can be almost any typical compression spring. AND, with the help of a friend here who's a MUCH better programmer than I, the model as assembled fills out the parts list properly (listing dimensions, different quantities, etc.). Now, if I have an assembly with a hundred different springs, it's really only one model stored in Windchill.

But, here's the problem with trying to do anything via a relation (I just tried it again per your suggestion but got the same result as when I tried it before.):

You cannot create a flexible item for a parameter driven by a relation.

http://support.ptc.com/help/creo/creo_pma/usascii/index.html#page/assembly%2Fasm%2Fasm_six_sub%2FTo_Define_Varied_Features_for_Flexibility.html%23wwconnect_header

IF it had worked I would have gotten around the problem you mentioned by limiting the choices for the materials to the ones we'd actually use.

Thanks for trying though!

The search continues....

P

pausob

Answer

19-Tanzanite

Well, before posting, I tried the technique I suggested and it worked on my system. But I'm still using Creo 2.0. Maybe this was "fixed" in later version.

And if "flexed" bolts work for your company - that's great! Do you guys use Windchill to report the BOM? Because I'd be curious as to how you manage to report the different bolt instances.

K

Kevin

1-Visitor

The only other option I see,besides the one already mentioned, is to use a family table.

Patriot_1776

Author

22-Sapphire II

.....which is how I handled it before in all my family-table fasteners, but in talking to the Windchill Admin yesterday he wants us to move away from family tables. I'm not sure I agree with the issues he says he's seeing (unauthorized people changing the table) because you can make the files read-only and make the Cabinet where the fasteners are stored as "Read Only", but, I think that's an uphill battle and I want to try something new anyway to limit the size of the gigantic table I have for my screws/bolts.

I'm going to put a ticket in with PTC and see if they can't find a solution. Not that I have much hope of that because in the past 23 years I cannot remember more than about 2 times they've actually been able to solve anything, but, for the outrageous sums they're charging for their yearly licenses now, I might as well put them to work....

I'll post if I find a solution.

Patriot_1776

Author

22-Sapphire II

Oh, and another reason I want to use real PTC materials, is that usually the Engineers that do FEA delete all the material properties of the assembly and instead assign them in Ansys (or Mechanica, etc.). I think that's a bad habit and the Windchill Admin agrees. We are moving away from that to prevent mistakes (assignment of the incorrect material in Ansys vs. the materials specified by the Design engineer). So, from now on, we're working to make EVERY part have the correct material at the creo level. One less possibility of a mistake. Plus, as I've found, there is Mechanica and even Ansys available inside of creo now (for a low, low extra price! - LOL).