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Using Windchill's Official Parameters with Repeat Regions

lhoogeveen
17-Peridot

Using Windchill's Official Parameters with Repeat Regions

I've been trying to figure out how to use PTC's Windchill parameters with Family Tables/Repeat Regions like any other parameters create by a user... but they seem to be hidden. Does anyone know how to use them with 1D or 2D repeat regions without using Relations to drive a new user parameter? It seems like PTC has either hid these on purpose or forgot about them completely. One would think PTC would give their own parameters equal/more preference not less... like not having to add them to a Family Table in order to use them on a Repeat Region.

PTC Parameters.jpg

Usually, parameters have to be in the Family table in order to use them in the Repeat Regions but the Windchill parameters cannot be added because they are hidden.

Family Table.jpg

Unable to Add Parameters.jpg

Repeat Region.jpg

12 REPLIES 12
TomU
23-Emerald IV
(To:lhoogeveen)

I'm not seeing any problem with a 1D repeat region.  (I have not tried a family table region.)

TomU
23-Emerald IV
(To:lhoogeveen)

I could be wrong, but I don't think you can display non-family table information on a family table repeat region.  I see what you mean about not being able to add PTC_* parameters to the family table.  Odd.

lhoogeveen
17-Peridot
(To:TomU)

Tom,

I think you're right... but it seems silly that I'm not able use Windchill parameters to the Family Table and thus unable to use them with Family Table Repeat Region. The only solution that I know of would be to drive a new parameter from the Windchill parameters through relations which adds complexity and method of failure if the relations get deleted.

I'm testing trying to using PTC_COMMON_NAME to replace our DESCRIPTION parameter (to allow changing descriptions from Rename/Save As in Windchill) and (unrelated) switching from a manual rev field to the Windchill Rev. I having a wonderful (terrible) time trying to get it to work Family Table Repeat Regions. I can get the PTC_COMMON_NAME to work with 1D repeat region but I end up having to create a hybrid 2D table since Common Name is treated differently than other Creo parameters. I can't seem to get the column order of the table to work properly in the 2D table.

Common Name - Family Table Repeat Regions.jpg

I tested using a DESCRIPTION=PTC_COMMON_NAME relation so I wouldn't need to redo the drawing tables but DESCRIPTION doesn't update in Windchill until the CAD has been checked in again.

I could open a case with PTC but they'll probably just give the well loved 'Works to Specification'.

Thanks,

Luke

BenLoosli
23-Emerald II
(To:lhoogeveen)

All Windchill parameters do not update until the file is checked in.

When we first implemented Windchill, our designers would model the part, then create a new drawing file and complain that their parameters were not correct. We had to remind them for a few months that the procedure said, Model, Save, Drawing, Save or Model, Save, Assemble, Save, Drawing, Save. Once they got that Save before doing something else with the file down, things worked a lot smoother.

We also discovered that we had to modify a lot of the PTC WM parameters to reformat them for something that we wanted in the drawing formats. We had to use local parameters that were extracts from the PTC_WM parameters. Dates in particular, since a PTC WM date includes a full time stamp and all we needed was the date of the year.

TomU
23-Emerald IV
(To:BenLoosli)

Ben Loosli‌,  Take a look at this:

CS49539 - "How can the date format for PTC_WM_CREATED_ON be customized in Creo Parametric"

Here's how we have it set:

date_type_parameter_format %yyyy-%mm-%dd

BenLoosli
23-Emerald II
(To:TomU)

My relations being extracted was originally done in Windchill/PDMLink V7 in 2005! I would hope where I used to work has updated the relation formatting since then. Maybe not, since they have switched to another CAD system when they were sold to another global parent. I know they still have some seats of Siemens NX and Creo for the legacy data, but it is not their primary tool today.

TomU
23-Emerald IV
(To:lhoogeveen)

I'm testing trying to using PTC_COMMON_NAME to replace our DESCRIPTION parameter...

Don't forget that PTC_COMMON_NAME is NOT versioned.  All versions of an object will display the same value.  On the other hand, DESCRIPTION most likely IS versioned (assuming it is a Windchill attribute tied to a corresponding Creo Parameter.)  This means the description for one version could be different from another version.  This is actually good if you don't want old (and potentially released) versions of a drawing changing their description after a rename (since rename affects ALL versions.)

lhoogeveen
17-Peridot
(To:TomU)

Ben Loosli

Agreed. Save the drawing is last is critical since we create our PDF's using the As Stored versions. Not always intuitive for the users since Creo will show the latest parts. We actually added an error during our Windchill promotion that if any of the drawing models have been modified without checking in the drawing, it won't promote the drawing. Catches users up occasionally but our data quality has much less errors of the two not being in sync.

Don't forget that PTC_COMMON_NAME is NOT versioned.

Tom Uminn Great point. Maybe it's best if I just link it DESCRIPTION = PTC_COMMON_NAME with a relation to be able to keep the older revisions the same. The objects would need to regenerated and checked in again in order to update the Windchill parameters. I could still see that relation updating old revisions of the drawing if that PDF got republished with Regeneration turned on. The DESCRIPTION parameter in Windchill would be the old description but the PDF would have the new description. We'd probably have to start using ModelCheck to make sure old objects get updated over time to include the relations. All in all, this is getting pretty complicated just to allow renaming the description from Windchill.

Another option might be to do some customization to Windchill/Creo to allow for batch updating of the Creo DESCRIPTION parameter that would just focus on the Latest objects or creating a new check in with the updated description.

TomU
23-Emerald IV
(To:lhoogeveen)

It would appear that the only non-family table parameter that can be used in a family table repeat region is PTC_COMMON_NAME.

What if you constructed an assembly containing each instance (just include) and then used an assembly region instead of a family table region?  Since all the instances are using the same names for the dimensions and parameters, you should be able to get a similar table.

llie
16-Pearl
(To:TomU)

All,

This be accomplished through the use of a relation added to your Creo start parts. We are starting to replace old parameters with relations that point to Windchill parameters to cut down on user input error. We can't eliminate the Creo Parameter name all together because we have so many legacy models that are reused in new assemblies. Here are two that we currently have in our start Creo start parts.

CAGECODE = PTC_ORGANIZATION_ID

TITLE = PTC_COMMON_NAME

BenLoosli
23-Emerald II
(To:llie)

When we migrated to Windchill, we had a custom modelcheck batch program constructed that would add the new relations to our files and remove out-dated ones.

We had a number of  parameters that we were adding, most being pulled from Windchill with modifications.

Copy of start part relations for a metric part.

/************************* START PART RELATIONS **********************
/* CALCULATE THE WEIGHT AND SURFACE AREA
/* --------------------------------------------------------------------------------------------------------------
/* YOU MUST DO A MASS PROPERTIES ANALYSIS AND THEN REGENERATE THE PART
/* FOR THE WEIGHT AND SURFACE AREA PARAMETERS TO BE UP-TO-DATE.
WEIGHT_KG = PRO_MP_MASS
WEIGHT_LB = PRO_MP_MASS * 2.20462
AREA_CM = PRO_MP_AREA / 100
AREA_IN = PRO_MP_AREA * 0.00155

/* SET PART NAME PARAMETERS FOR BOM
/* ------------------------------------------------------
/* PART_NO  PARAMETER  IS ALWAYS EQUAL TO THE MODEL NAME.
PART_NO = EXTRACT(REL_MODEL_NAME(),1,8)

/* DWG_NO PARAMETER IS ALWAYS EQUAL TO PART_NO
/* IF THEY ARE NOT, COMMENT THIS RELATION
DWG_NO = PART_NO

/* extract the date portion of the windchill timestamp params
short_created_on = extract(ptc_wm_created_on,1,10)
short_approved_date = extract(ir_approved_date,1,10)
short_modified_on = extract(ptc_wm_modified_on,1,10)
year = extract(ptc_wm_modified_on,1,4)

/* Set initial_ecn = to ecn from windchill only when rev is 0
if ptc_wm_revision == "0"
initial_ecn = ecn
initial_created_by = ptc_wm_created_by
initial_created_on = short_created_on
endif
/************************* COMPONENT RELATIONS ***********************

TomU
23-Emerald IV
(To:llie)

We can't eliminate the Creo Parameter name all together because we have so many legacy models that are reused in new assemblies.

This be accomplished through the use of a relation added to your Creo start parts.

Are you having your users manually add these relations every time they open an old part or are you doing something with ModelCheck?

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