Excluding Component From Windchill BOM Structure

[Matt_C]

Version: Windchill 11.2

Use Case: Wondering if there is a way to tell Creo/Windchill that a component in an assembly is not to show in the BOM structure.

Description:

I am trying to get an accurate BOM to take directly to Syspro MRP. We don't use WT parts at this time so looking for a solution without WT parts if possible. We currently export a CSV of the multi-level structure report from Windchill and import this into Syspro. This method works great until we have components in the CAD assembly that we don't want to show in Syspro. Then we have to manually go through and clean things up. Would be great if a part could be set to not show in the BOM- whether that is from within Creo or within Windchill . We use Creo 8.0.10.0 and Windchill 11.2.1.0

Thanks!

Matt

[joe_morton · Accepted solution]

Not sure if this is actually easier, but you could:

• Add a feature parameter ("Feat Params") to your model tree
  • I'd set it as a "Yes No"
  • Make sure to mark it as "Designated" -> this means it will get sent to Windchill
  • Probably want to add this to your Assembly templates to ensure it's consistent
• Engineers would then mark the parts to exclude using this parameter
• In Windchill, you'll need to map the new feature parameter to CAD Document Uses Link attribute
  • Create a new attribute with the same internal name as what you named the parameter in Creo
• From there, you'd include the new attribute in your CSV exports and you'd have the additional step of filtering on that attribute before uploading to Syspro

[Matt_C]

I will look into this, thanks! Few questions:

---

@joe_morton wrote:Probably want to add this to your Assembly templates to ensure it's consistent

---

 What exactly would I be adding to the assembly start part? 

If my parameter is called something like "SYSPRO_BOM" for example, is there a way to make so all parts are by default "Yes" by using the assembly start part?

What about for existing assemblies- is there a good way to set the parameter without having to do every part individually? 

Or what about if this feat param is only set to "No" for a couple items in the BOM, the rest being unset, will the Windchill attribute show up blank and after exporting could we filter out any items with the value of "No" ?

Based on your response I was able to find a few more forum posts on this topic so I will do some more reading too. 

[joe_morton]

You'd want to add that new feature parameter to the assembly start part. Otherwise, everyone has to add it manually and if they type it wrong, it won't update Windchill correctly.

For existing assemblies, I don't think there's a good way to do it. You have to open Creo, add the feature parameter, then update each part that needs to be excluded. It may be tempting to just update the value in Windchill directly, but the next time the Creo model is checked in, it may wipe out the values.

Yeah, using SYSPRO_BOM, I would have yes/no, where I'd only filter out the "no's". Yes and blank would all stay in the BOM. 

[Matt_C]

I may be missing something here, but that parameter is showing up in as a model tree column for new assemblies now, even though I didn't add it to the start part. Is the issue just when there's multiple users involved? 

I created the Windchill attribute by following the instructions in this post:

https://community.ptc.com/t5/Windchill/Add-Attribute-to-CAD-Document/m-p/494664/highlight/true#M52920

The attribute/parameter is now available in Windchill, but after I set the value to yes/no for a few different components in an assembly, checked the assembly back into Windchill, nothing shows in the table:

Any ideas on what I did wrong? 

Thanks!

Matt

[avillanueva]

Is the attribute designated?

[Matt_C]

Yes I believe the parameter is designated in Creo. 

Thanks!

[joe_morton]

Yeah, you'll see the new attribute everywhere, with all the values blank. When you check in a Creo assembly that has values (yes or no), the structure in Windchill should update accordingly. 

[Matt_C]

Problem is, I did check the assembly in but the structure did not update.... 

[Matt_C]

Figured I would run a test and share the pics of the steps I'm taking to make sure I'm not doing something incorrectly. 

New test asm, brought in 2 parts:

I click in the (highlighted blue) cell for "SYSPRO_BOM" parameter. Parameter properties window opens. Here's the defaults:

Parameter properties, after I make the changes I want:

Model tree shows the parameter value "NO":

Check in: 

Nothing shows up in Windchill: 

[BenLoosli]

Is the internal name in Windchill for your new attribute in CAPITAL LETTERS?

The parameter will not sync with Windchill even if designated if the internal is not capital letters.

[Matt_C]

Yes it is. Thank you for checking.

[joe_morton]

I think I see the issue.. you set the Windchill attribute to String, but in Creo, it's "Yes/No". So change Windchill to be a boolean. I don't think you can change the type. You'll probably need to delete it and recreate it.

[Matt_C]

Good catch! That was partly the issue. I also had added the attribute under Type CAD Document instead of Type CAD Document Uses Link... didn't realize the difference there. After making both of those changes it seems to be working now. 

Thanks again,

Matt