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ptc-52803111-Visitor
1-Visitor
May 20, 2014
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Relations Between Multiple Parts

  • May 20, 2014
  • 5 replies
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I am working on creating an electric motor assembly that will adjust based on given parameters. For example I want to be able to adjust the rotor lamination and have the rest of the assembly adjust accordingly. The issue that I am currently running into is I am not sure how to create relations between seperate parts. Is there a way to do this in Creo 2.0?

Thanks


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    Best answer by TomU

    Definitely! There are multiple ways to do this. Probably the easiest is to simply create the necessary parameters in the top level assembly and then let the individual parts read them from this assembly. To keep things more robust, I'd recommend you recreate the relevant parameters in each part and then simply use the value from read from the assembly to set the part's parameter(s). This make it much easier to 'turn off' the top level assembly control when you want to make sure the part is behaving correctly.

    To read parameters (or dimensions) from another model in an assembly, you have to use the parameter name (or dimension) followed by the session ID. For example, if the top level assembly has a parameter named "ASMPARAM" and, part has a parameter named "PRTPARAM", and the assembly has a session ID of "25", the syntax would be this:

    PRTPARAM = ASMPARAM:25

    You can find the session ID by going to Tools/Relations (while in an assembly) and clicking on Show/Session ID.

    5 replies

    D
    dschenken1-Visitor
    1-Visitor
    May 20, 2014

    There's a module that is called Layout in WFx, not sure what the Creo name for it is. It is a 2D sketch location that allows multiple parts and assemblies to access a common set of dimensions and other values. Think of it as a cocktail napkin quality sketch with the important values on it.

    I know there is a NEW! ALL NEW! CREO! Layout module, but I don't know if it's the same central information repository that it is under WFx.

    Also formerly known as Pro/Notebook, I believe.

    T
    23-Emerald IV
    TomU23-Emerald IVAnswer
    23-Emerald IV
    May 20, 2014

    Definitely! There are multiple ways to do this. Probably the easiest is to simply create the necessary parameters in the top level assembly and then let the individual parts read them from this assembly. To keep things more robust, I'd recommend you recreate the relevant parameters in each part and then simply use the value from read from the assembly to set the part's parameter(s). This make it much easier to 'turn off' the top level assembly control when you want to make sure the part is behaving correctly.

    To read parameters (or dimensions) from another model in an assembly, you have to use the parameter name (or dimension) followed by the session ID. For example, if the top level assembly has a parameter named "ASMPARAM" and, part has a parameter named "PRTPARAM", and the assembly has a session ID of "25", the syntax would be this:

    PRTPARAM = ASMPARAM:25

    You can find the session ID by going to Tools/Relations (while in an assembly) and clicking on Show/Session ID.

    D
    dgschaefer21-Topaz II
    21-Topaz II
    May 21, 2014

    You can do so, as Tom described, but I'd suggest you search the PTC knoledge base and other sources for information on skeleton based top down design. A bit complex, but extremely powereful and designed for exactly what you are tying to do.

    T
    23-Emerald IV
    TomU23-Emerald IV
    23-Emerald IV
    May 22, 2014

    Doug Schaefer wrote:

    You can do so, as Tom described, but I'd suggest you search the PTC knoledge base and other sources for information on skeleton based top down design. A bit complex, but extremely powereful and designed for exactly what you are tying to do.

    I could be wrong, but I'm pretty sure you still need to create your relations to the skeleton parameters the same way you would to any other assembly/part. In this case, you're just choosing to refer to the skeleton part's parameters instead of the top level assembly's parameters.

    D
    dgschaefer21-Topaz II
    21-Topaz II
    May 22, 2014

    Tom Uminn wrote:

    I could be wrong, but I'm pretty sure you still need to create your relations to the skeleton parameters the same way you would to any other assembly/part. In this case, you're just choosing to refer to the skeleton part's parameters instead of the top level assembly's parameters.

    I made the assumption that the "parameters" he intended to drive could be expressed in the actual geometry, in which case you would not need any relations. However, if they are non geometry values that are indeed stored in Creo / Proe parameters, then you are correct.

    J
    Jeroen1-Visitor
    1-Visitor
    May 22, 2014

    We use this the whole time.

    Clipboard01.jpg

    Some rules:

    The most interesting place to put the relations between an assembly and a part (or subassembly) in that assembly is in the component. This way the relations won't fail if you suppress the part for some reason, and you will still be able to open and edit the part without the assembly in memory.

    A good practice is to use parameters in each part/assembly, and to write relations between these parameters.

    To write a relation, you don't need to search for feature-ID's and component ID's. Creo will do that for you. Just click on the button to 'Insert Parameter Name from List', and select the part you want to see the parameters from. Creo will add the correct ID's by itself.

    P
    ptc-52803111-VisitorAuthor
    1-Visitor
    May 22, 2014

    I am just wondering if I were to put the parameters in each of the individual components how can I use the parameters in multiple parts. For example the motor that I am trying to modify will change in length. The length will change most of the parts in the assembly. However, I do not want to have to go to each individual component to change the parameters. Is there a way to do this with a spreadsheet that parameters would read from or.....??

    Thanks,

    Brad

    D
    dschenken1-Visitor
    1-Visitor
    May 22, 2014

    This is what the Layout tool does.

    There used to be a poseable human-like figure model based on layout that had a table that drove poses.

    J
    jmayer1-Visitor
    1-Visitor
    May 22, 2014

    A notebook can be used to store all of your parameters and relations in one place. All of your parts can point to the notebook (declare is the command I think). If the values in the notebook change, the parts will change as well.

    The parameters can be placed in table format to make modifying similar to using excel.

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