Master Model Approach. UGMaster vs. UGPart file name, pros/cons?

[apekim]

The Siemens integration guide suggests to use the master model approach. The guide suggests to first create your part (UGMaster dataset); this part is stored in the item revision in Teamcenter. Next, the guide suggests to create a UGPart dataset and add the UGMaster dataset to it as a component (the same way you build an assembly). The guide mentions that the UGPart dataset is stored in the same item revision as the UGMaster dataset. The guide suggests to create the drawing in the UGPart dataset, and not the UGMaster dataset.

Question regarding above info: Would the item number of the UGPart be the same as the item number of the UGMaster? Is this even possible?

Prior to reading the Siemens guide, my understanding was that the suggested technique was to create a separate item for the drawing which would be just the basic part number. (Example: 12345-1.prt for the part and 12345.prt for the drawing.

It seems you can do this three different ways. If you need to add a document to a parts list to be delivered with the unit, is it required that a separate "basic part number" item be created for the drawing?

Thanks,
Mike

 

[MickyV007]

Have a look at att. example maybey it clears somethings out. Don't mention the TB attributes note at the bottom.
We have called our drawing (=specification) 110-01, or 190-01 or ... all beneath an item revision. In Tc you can add multiple other datasets like an excell sheet under the item revision. The item revisions are all part of the top item (=big red knot).

Best regards,

Michaël.

NX4+TC9 / NX6+TC8Unified / NX7.5 native

 

[apekim]

Michael,
Thanks for the reply.

I took a look at the image you had attached. What version of Teamcenter and NX are you using?

How is the drawing added to the item revision? Is 110-01 the Item ID or the item Name (description).

In some cases we may have a need to deliver a drawing along with the product. In this case I would need to add the drawing to the parts list with a qty of 1. I dont think I could do this if it is set up like yours. Do you agree?

Mike

 

[MickyV007]

Mike ,

we still use TC9 but already working on shifting to TC8 Unified + NX7.5. The look and feel of the TC8 is completly different prior to TC9. But the principle stays the same.

As for the drawing; it is created wihtin NX with NX manager as a specification beneath the item revision, so the 110-01 is the item name.
3222-021-2949 = item
3222-021-2949/1-01 = item revision
and if you preform an export of your part and drawing out of teamcenter the drawing would look like this
3222-021-2949-110-01.
Only within TC it is presented to you simplified like 110-01.

When you're using master model approach and you need to provide a customer or supplier with the model and drawing then you have two UG parts (one=master and one=spec) if exporting the item out of TC.
Our sysadmin has written an automated function within NX to preform this kind of export, it also creates a step and parasolid file.

Example attached.


Best regards,

Michaël.

NX4+TC9 / NX6+TC8Unified / NX7.5 native

 

[apekim]

So when you create the drawing, you do not assign it an Item ID (Part Number) to it?

How do you handle part families or part variations which are identified on a single drawing using a table:
In some cases these families of parts are either created as a part family or as stand alone parts...either way they would be controlled by a single detail drawing. We create stand alone parts when we design opposite hand parts that may have many features. It is usually too involved to use part families for these.

Also, In some cases we need to ship a copy of a document in the shipping box, along with the assembly. I can't see how this would be done using your method because when you add the item revision to the parts list it will add the item to the bomview.

This is good info to understand...Thanks!
Mike

 

[MickyV007]

Mike,

now i see your problem. We sometimes also deal with this kind of difficult constructions. The way we solve at the factory is create a part family from the original codenumber/part and create seperate numbers (=items/parts) for different kind of production steps, so we have a part/codenumber for the product that comes from the supplier/customer and then we create a family table with it.
Then we have an excell table (on a network server) in which we can create different codenumbers (accessable for every mechanical desginer). In NX we use this number as a new part/assembly and place the correct family member beneath it, then you can create a drawing there also using the master model concept and still have the link with the original part.

So lets say we buy a 3222-...-..../1-01 number as component an process it on different machines, then we create 7204-...-..../1-01 numbers for each neccessary production step and place a member of the part family from those 3222 number beneath those 7204 numbers and so we can create the drawings for those prdo (master/model).
Need a point number increase no problem. Do a save as from 3222-...-..../1-01 into 3222-...-..../2-01 and create the family table again, everywhere those members are used they are updated automaticly.

Maybey this clarifies some things out.

Best regards,

Michaël.

NX4+TC9 / NX6+TC8Unified / NX7.5 native

 

[apekim]

Michael,

Please see the attached pdf file. On the left you will see 2 options for storing NX cad datasets. We need to decide on one of these 2 options. I am searching for pros and cons of each.

Or the right you will see 2 different methods of storing parts which are detailed on the same detail drawing. For both ways the detail drawing will have a variant table for each of the 5 similar parts. The table may define different dimension lengths (1.0", 1.5", 2.0", 2.5", 3.0") for dimension "A" on the drawing. Depending on the complexity of the model, these parts can either be in a part family or modeled as separate parts. Because of the lower scenario, it would make sense for us to store the CAD drawing in a separate item/item revision (option #2 on the left). But I am open to look at other ideas.

Mike

Mike

 

[MickyV007]

Mike,

you could choose option #1 (master/model concept) and when creating the NX DRAWING place the according member of the family table in the drawing.
Just like in an assy you can substitute the part in the specification. Then there will also be a direct link to the original item.
Let's say a wire is cut in different lengths like in your example (1.",1.5",..., and so on).
If you store (create) all these parts in seperate items and somehow the diameter of the original part changes, then you need to open every item and change the diameter in all these items, so there's a change you forget one or make a mistake.
When you choose for option#1 then you place member A with length A beneath drawing 110-A, member B with length B beneath drawing 110-B, and so on. Changing the diameter of the wire is done in one place, namely the template (=item) and then update your family table with the result that all your drawings will be updated automaticly.

Anyhow, these decisions are always hard to make, its good to have a good thought about it before you begin. Depending on the complexity of your products and interaction with clients/suppliers you should make an acceptable choice for every party.

Best regards,

Michaël.

NX4+TC9 / NX6+TC8Unified / NX7.5 native