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Relations Between Multiple Parts

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Relations Between Multiple Parts

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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Accepted Solutions

Re: Relations Between Multiple Parts

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.

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25 REPLIES 25

Re: Relations Between Multiple Parts

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.

Re: Relations Between Multiple Parts

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.

View solution in original post

Re: Relations Between Multiple Parts

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.

--
Doug Schaefer | Engineering Manager
Crow Works

Re: Relations Between Multiple Parts

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.

Re: Relations Between Multiple Parts

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

Re: Relations Between Multiple Parts

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.

Re: Relations Between Multiple Parts

Would you have an example of a layout or know of somewhere that I could get a tututorial on it? I am a little nervous to try the layout as I have never worked with it before.

Thanks,

Brad

Re: Relations Between Multiple Parts

I'd suggest the help topics under large assembly management - at least that's where it is described for WF5.

They are easier to use than most everything else. Lack of familiarity is the main problem - under the best circumstance one would create a single layout that could drive thousands of models and never have to modify the layout again, leaving one with the feeling that layouts are 1/1000th as usable as models, when the opposite is true.

Layouts are the Rodney Dangerfield of parametric modeling.

Re: Relations Between Multiple Parts

The way I would do it:

- Create the parameter "LENGTH" in every part/subassy you need it in.

- Let this parameter drive the feature that needs the length (feature relation like "d14 = LENGTH"

- Create the parameter "LENGTH" also in the main assy

- Create the relations to all parameters. This can be don in the main assembly relations, or in the components, or in the parts. You're free to choose, every location has it's pro's and cons.

This would look something like:

LENGTH:0 = LENGTH

LENGTH:2 = LENGTH

LENGTH:4 = LENGTH

you can also add some more intelligence like

if LENGTH > 100

LENGTH:6 = LENGTH * 1.1

else

LENGTH:6 = LENGTH + 5

endif

- Now you can alter the parameter LENGTH in the main assembly, and everything will follow.