23-Emerald IV

Question

Managing Variation (Windchill, Creo, and ERP System)

Forum|Forum|11 years ago
August 29, 2014
7 replies
1827 views

Cross posting this from the PTC community.

So far I kind of like option 5, but I’m not sure how tough it will be to actually implement.

Thanks!

Tom U.

Other

D

davehaigh

13-Aquamarine

This doesn’t apply directly to what your question is but it talks about using family tables strictly for parameter information.
This was put together in Wildfire 1, so be advised. I’m not sure I’d recommend going down this path. Hopefully someone has something better to suggest.

Pro/E

Assembly Issues

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Assembly Drawings
There is no good way to create Assembly drawings for manufacturing where the assemblies needed do not correspond to the existing assemblies in the model. Almost all the upper level assemblies for the CLS have these issues.

Our solution:
A simple example will help explain the issue, lets say that in our design assembly we have two sub-assemblies and a number of parts, but for manufacturing purposes we want three assembly drawings for this section of our machine.

Simplified Reps to include components
The first thing to do is create three simplified reps inside the design assembly, using exclude all. Then include just the parts you want for each one of the three assembly drawings.

Family Tables to control parameters
The problem you now have to solve is how to get different title block information for each of the three drawings. You do this by creating a family table in the assembly that includes only the parameters you need for your title block and BOM. So in our example, we would have a family table with the generic and three additional instances.

It is important that you don't try to eliminate or include components within the family table. Use the simplified reps to do that, otherwise the combination of simplified reps and family table can get confusing very quickly.

Modifying the Title Block and BOM
You can now create the assembly drawings using the correct simplified rep for that particular drawing. To get the correct info in the title block you pick File, Properties, Drawing Models, Replace, and select the family table instance that corresponds to simplified rep. To update the BOM pick Table, Repeat Region, Model/Rep and pick the assembly the family table instance, and the simplified rep that are related to this assembly drawing.

Use Partial Views to limit view extents
Many of the models have large extents compared to the geometry. Make all the views partial views and just sketch the boundary around the outside of the geometry. This keeps the views from overlapping.

Explode States
Exploded view states should be named so it is fairly obvious in which drawing and view they are used. At this point there is no naming convention for these. I would suggest that you standardize on a naming convention for simplified reps, explode states, and family tables. All three relate to assembly drawings as we do them and should likely include the drawing number and a description in the name.

Calling out these non-assemblies in upper level drawings
Finally there is the issue of how to call out these fake assemblies, in the BOM of an upper level assembly drawing. This is an issue because they do not exist as actual Pro/E assemblies and have no parameters that would fill in the BOM in the upper level assembly drawing.

In some cases we used bulk items in the higher level assemblies. In other cases we just added a row or two to the table, typically item #1, and filled in the information manually. This can cause a problem if you go back and change the name of one of the sub-assembly drawings, because this information is not associative. That’s true for the both the bulk items and the manually entered data.

Issues with this method
Issues with this method are that if you go back, and either add parts to the assembly, or replace parts in the assembly, it is likely that they will not show up in your views or BOM. You will need to go back and redefine each of the simplified reps to include the new items. The behavior seems to be sporadic. Sometimes you see the parts sometimes you don’t. It seems to be dependent on which assembly or sub-assembly they were added to. For example if you included an entire sub-assembly in your simplified rep. Then the parts added to that sub-assembly would likely show up. But if you only added some models in a sub-assembly to your simplified rep. Then the new parts would not show up.

You need to pay extra careful attention to the BOM and BOM balloons on assembly drawings.

The same caveat holds true for explode states in your assembly drawing. Adding or replacing parts in an assembly will adversely affect your explode states and offset lines. You need to go back over those views carefully.

Memory limit issues with large assembly drawings
There is an issue with using drawing templates when creating drawings of large assemblies. If you don’t use the template file, when you place the first view of an assembly on a drawing, Pro/E asks you if you want to use a specific simplified rep of the assembly. If you use the template file for your drawing, Pro/E will not ask you for a simplified rep, but will try to place the master rep into the drawing. With a number of our top level assemblies, this behavior will cause your system to crash. The alternative with these assemblies is to not use the template and manually run the drawing program as described in this link.

For smaller assembly drawing use the drawing template, but after the master rep is placed, then pick view properties and “Change View State”. This will bring up a window that will allow you to select the simplified rep you wanted. Once you have done this for the first view, all other views you add to the drawing will default to that simplified rep.

You can use “Change View State” to change which simplified rep is used in a specific view of a drawing. Drawing AD001234 is a good example. Each view is a different simplified rep and explode state.

BOM issues with assembly drawings
Doing assembly drawings the way we have there are a number of issues with creating the BOM on the assembly drawing.
1.You most often need to set the repeat region attributes to recursive.
2.You will need to filter out a lot of items that you don’t want to show in the BOM
3.Sometimes filter by item does not work on some of the rows in the BOM. When this happens there are several reasons why a row will not filter.
a.There are multiple models that have the same parameters.
b.There are family table instances that have the same parameters.
You solve this by filtering by rule. There are two parameters you can write a rule on. &asm.mbr.part_num or &asm.mbr.drawing_title4. A typical filter rule would look like this &asm.mbr.part_num!=AD001234
Where AD001234 is the drawing number in the row you don’t want to see.

All the BOM’s should be “fixed” so that the numbers do not move around as you add and remove components from the assembly. The BOM order should be as follows.
1. All Lyncean manufactured components, in the order of assembly, or grouped by type.
2. All purchased components, beginning with major components such as slides, motors, flanges, etc., and ending with fasteners. All fasteners should be grouped by type. For example all socket head cap screws, from smallest to largest. All hex head screws from smallest to largest. All washers from smallest to largest, all nuts from smallest to largest, etc……

Layers in drawings
Turn off all layers in drawings except for the Gtols and Notes layers. Be sure and save this layer state.

Layers in parts and assemblies
Turn off all layers in all parts and assemblies and save that state. Always remove “set datums” and axes to the datums and axes layers and place them in the Gtol layer. This is done using cut and past in the layer window.

Assemblies Templates
There are multiple assembly templates. The idea behind this was to be able to access the default datums for each assembly separately. I doubt that this is necessary with the new layer interface in Wildfire. It made more sense in 2001 and prior releases.

David Haigh

S

SS_10717305

5-Regular Member

Create a configurable Module / product in Creo Parametric
Create a module variants in Creo parametric
Define Refrence Pairing
By simply check-in with auto-associate user would get configurable WTPart structure
Define Options and Choices in Windchill. Also can set business rule for module variant
Create a Variant specification in Windchill
Create a Product variant in Windchill
Publish the product variant to ERP system.

This requires Creo Parametric Options Modeler, Windchill ATO Capability and ESI for Windchill BOM Publishing to ERP.

Thanks,

Shakil

MarcoTosin

21-Topaz I

Tom,

look at this discussion on PTC community.

http://communities.ptc.com/thread/55427

Marco

T

TomU

Author

23-Emerald IV

Shakil,

Can you please clarify the first couple of steps? From looking at the help documentation a 'configurable module' is "an assembly ... that supports multiple design variations". In this particular case, I need the variation only at the drawing, or possibly CAD part level. There are no assemblies involved in the variations.

1 CAD model/drawing == multiple Windchill part numbers, each with their own unique representation of the same cad, but displaying different materials (probably watermarked).

Thanks.

Tom U.

S

SS_10717305

5-Regular Member

Hi Tom,

In your case, is only material variation in product variant?

Below approach help both variation in form, fit, or function and material.

Not sure you’re only goal is to deal with business use case where design is same and only material is different, which I feel NOT the only change in product variant right?

Thanks,

Shakil

T

TomU

Author

23-Emerald IV

"Not sure you're only goal is to deal with business use case where design is same and only material is different, which I feel NOT the only change in product variant right?"

No, the ONLY change is material (or hardness, or coating). No changes to form, fit, or function. No changes in CAD (preferably). No changes in CAD assemblies.

I'm trying to capture options chosen at order time without unnecessary duplication in the CAD system. In some ways "material" is no different than "due date", "vendor", or "order quantity", except everyone expects it to be on the drawing.

Make sense?

C

cc-2

1-Visitor

Hi

many suggestions were made that I will not repeat. I have not seen thought about using Inheritance. This allows you to create a new model (so new number) while been dependent on the inherited one. So if one change the other will change too.

As someone said, I think, (sorry I did not read all in details), you can also work only with the wtpart and use the same CAD in all the different wtpart.

We have something similar in our company where the same component (same dimensions) will have variation (such as different raw material if it is made in EU or in China), we create 2 different model (with inheritance dependency).

In the assembly which can use either we use Replacement Parts. so assembly made in EU will use the pin from the EU and the assembly (same partnumber) made in China will use the chinese pin.

Hope this helps

Best regards

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