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Create part name in a note

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Create part name in a note

How can I get the part name in a note? I have tried &model_name, but then the name of the assembly is displayed.

Knipsel.PNG

1 ACCEPTED SOLUTION

Accepted Solutions
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Re: Create part name in a note

Another way to do this is to find the part's session id.

Open the relations dialog (Tools tab > relations) and then pick Show > Session ID, pick Park in the pop up menu and then pick the part in question on screen. The session ID will be shown in the message area. Then create a note with this text '&model_name:ID where ID is the number you just found.

Another method would be to create a user parameter in your part tied to the file name. Enter the relation file_name = rel_model_name in the part's relation and then use &file_name:att in your note attached to the model.

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Doug Schaefer | Experienced Mechanical Design Engineer
LinkedIn

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15 REPLIES 15
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Re: Create part name in a note

If your note is attached to the edge of the model in question (and not an edge created by a section, for example), you shoudl be abel to use &model_name:att).

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Doug Schaefer | Experienced Mechanical Design Engineer
LinkedIn
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Re: Create part name in a note

Doug,

Is the ":att" the number of the model in the assembly? How do you find that number?

Thanks, Dale

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Re: Create part name in a note

Doug,

Ik cut and paste your command in my note, but it doesn't work. I have selected on entity and on surface. Knipsel.PNG

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Re: Create part name in a note

Off the top of my head I believe the syntax is: &model_name:att_mdl

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Re: Create part name in a note

Hmm, I've always used the ':att' suffix and it has worked. Proe / Creo will convert it to :att_mdl.

I just tried both in Creo 2 and they don't work. Opened the same drawing in WF4 and it didn't work there either.

I tried it again using a user created parameter and it worked fine. I guess it doesn't work with system parameters. Odd.

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Doug Schaefer | Experienced Mechanical Design Engineer
LinkedIn
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Re: Create part name in a note

Another way to do this is to find the part's session id.

Open the relations dialog (Tools tab > relations) and then pick Show > Session ID, pick Park in the pop up menu and then pick the part in question on screen. The session ID will be shown in the message area. Then create a note with this text '&model_name:ID where ID is the number you just found.

Another method would be to create a user parameter in your part tied to the file name. Enter the relation file_name = rel_model_name in the part's relation and then use &file_name:att in your note attached to the model.

--
Doug Schaefer | Experienced Mechanical Design Engineer
LinkedIn

View solution in original post

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Re: Create part name in a note

Doug!

It works, thank you!

Knipsel.PNG

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Re: Create part name in a note

What method did you use - the ID?

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Re: Create part name in a note

Hi,

...if I need to check the corect information "att_mdl" for note in drawing - I create "fake relation" in assembly mode - system automatically create for me information (behind parameter in relation) and then I can use this number to my note in drawing

For example:

note.JPG

Best Regards,
Vladimir Palffy
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Re: Create part name in a note

Now I have made a "mapkey" to search for the session ID. In the mapkey is also the command for making the note. It takes seconds to place the part numbers in a assembly.

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Re: Create part name in a note

I like mapkeys too -

Here is some Trisks with Mapkeys and video Hide custom Layers with Mapkeys

Best Regards,
Vladimir Palffy
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Re: Create part name in a note

Nice! Personally, I would have gone with the parameter & relation so that the note is tied to the part it's attached to but either way works.

BTW - I have a good friend named Stefon Lowman.

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Doug Schaefer | Experienced Mechanical Design Engineer
LinkedIn
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Re: Create part name in a note

don't mean to thread hijack 😉

is there something similar for zone locators?

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Re: Create part name in a note

I have created idea for new release

What do you think? Vote here: Enable Show/Hide Session ID in Model Tree

Best Regards,
Vladimir Palffy
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Re: Create part name in a note

For some reason I have found that I have to enter the parameter in lowercase &model_name and uppercase &MODEL_NAME does not work. For multi-part drawings, whatever model I have active, ProE / Creo will append the correct number at the end e.g. &model_name:12

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