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Andrew_41012-Amethyst
12-Amethyst
March 28, 2025
Solved

Assigning material properties to bulk items in Creo 2.0

  • March 28, 2025
  • 3 replies
  • 1555 views

I'm using Creo 2.0 currently and would like to be able to assign material properties to bulk items in an assembly I have. I want this for reporting the PTC_MATERIAL_NAME parameter in my drawing BOM. In the assembly model in Creo 2.0, there's no way to right-click on a part and assign materials. For each part, I have to open them and manually set the material by going to File -> Prepare -> Model Properties, which is not an option for bulk materials because the only way to access them is through the Relations window. PTC_MATERIAL_NAME is a reserved parameter and cannot be manually added in relations.

 

Do I need to change my BOM settings to a user defined parameter for each part in the model? Any other workaround?

Best answer by KenFarley

There's a trick I use to be able to include a part in an assembly without actually adding the part. For example, say I have a fixture I need to include in an assembly to allow a person to build the thing. I don't want to actually have the fixture assembled as a solid model. That would botch up the mass calculations, etc. To do this I do the following:

(1) Create the part or assembly as usual, fully defined. Set its parameters or in your case material properties appropriately.

(2) Add a family table to the part or assembly.

(3) Add a column or columns to the family table for the first feature.

(4) Add an instance to the family table for the bulk item. I.e. if I'm doing this with a part called "drill-fixture" I will name the instance something like "drill-fixture-bulk".

(5) Enter a "N" in the column of the first feature for this bulk item.

(6) Assemble the instance into my assembly. Creo will give a warning that I'm adding an empty part, which is exactly what I want it to do.

 

Now the Bill of Materials will list the pseudo-bulk item. I do this so if I change any of the drawing-relevant information of the "real" part, it will be reflected in the "bulk" instance of that part. Which happens surprisingly more often than one would think. 

 

Maybe this technique will work for you.

3 replies

K
KenFarley21-Topaz IIAnswer
21-Topaz II
March 29, 2025

There's a trick I use to be able to include a part in an assembly without actually adding the part. For example, say I have a fixture I need to include in an assembly to allow a person to build the thing. I don't want to actually have the fixture assembled as a solid model. That would botch up the mass calculations, etc. To do this I do the following:

(1) Create the part or assembly as usual, fully defined. Set its parameters or in your case material properties appropriately.

(2) Add a family table to the part or assembly.

(3) Add a column or columns to the family table for the first feature.

(4) Add an instance to the family table for the bulk item. I.e. if I'm doing this with a part called "drill-fixture" I will name the instance something like "drill-fixture-bulk".

(5) Enter a "N" in the column of the first feature for this bulk item.

(6) Assemble the instance into my assembly. Creo will give a warning that I'm adding an empty part, which is exactly what I want it to do.

 

Now the Bill of Materials will list the pseudo-bulk item. I do this so if I change any of the drawing-relevant information of the "real" part, it will be reflected in the "bulk" instance of that part. Which happens surprisingly more often than one would think. 

 

Maybe this technique will work for you.

    P
    Patriot_177622-Sapphire II
    22-Sapphire II
    April 2, 2025

    'Sup Ken!

     

    Here's a thought:  Export the drill fixture assembly out as a STEP model, use a skeleton part in your real assembly with the drill fixture as solid or surface import into your skeleton model.  As I remember, skeleton parts are automatically filtered out of BOM's but you should still be able to show it visually in the dwg.  Haven't played with that in a while, but I think so.  Also, if the drill fixture changes, you can re-import it.

    K
    KenFarley21-Topaz II
    21-Topaz II
    April 3, 2025

    Hi Frank,

    The thing is, I want the exact opposite of this. I want the fixture to show up in the Bill of Materials, but I don't want it to be represented any way in the actual model. The equivalent of a bulk item, but more what might be called a "ghost component". By using an instance of the actual fixture that has no geometry, I get all the parameters of the fixture but none of the geometric overhead. It works nice. A bit of setup required on the front end, but well worth it.

    P
    Patriot_177622-Sapphire II
    22-Sapphire II
    March 29, 2025

    I never use the "bulk" parts, I find them too restricting.  What I do is use a regular start part as the starting point and have a relation to set a parameter in there to fill out the BOM as "AR" quantity.  Or, you could even make it say "10 fluid Oz.", etc.  I then constrain it at assembly in the default location.  This way, say, if it's a lubricant or adhesive etc. that needs to be applied to a specific area(s), I copy the surface(s) from whatever part(s) at the assy level into the "bulk" part and then I can point an item balloon to that and assign a flagnote to it saying "APPLY ITEM XX TO SURFACE(S) SHOWN." or similar.  In the case of the "bulk" item needing to be applied to several surfaces, you can also add ref balloons.  Since you're starting with a regular start part, you can then make it a family table "bulk" part to have, say, different viscosities (and BOM descriptions) for oil, different colors or types of paint etc.  Works out really well, the only downside is now there is a link from the assy and part(s) to that "bulk" part, but as long as you're careful and don't create circular refs, you're good.

    A
    aputman13-Aquamarine
    13-Aquamarine
    April 1, 2025

    Add the bulk item to an assembly, expand it out until you see the body of the bulk item, right click on the body and Assign Material. 

    Edit:  Just realized you said Creo 2.0.  Not sure if this would be supported. 

    aputman_0-1743544996123.png

     

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      Andrew_41012-AmethystAuthor
      12-Amethyst
      March 16, 2026

      This indeed is not a feature of Creo 2.0. However, I'm now working in Creo 11.0.6 and still do not see the option to expand bulk items out, right-click, and assign materials. By right-clicking it within the model tree, I have options to move, suppress, replace, open, etc., though no options to expand and right-click bodies for assigning materials. Opening a bulk material leads me to its relations/parameters window where I still can't update the material. 

      Screenshot 2026-03-16 180208.png

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      aputman13-Aquamarine
      13-Aquamarine
      March 17, 2026

      If that is a bulk part that was created in 2.0, maybe try creating a new bulk item and see if the option becomes available. 

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