Find all Part ID numbers in Creo Drawing

[al3]

I have a drawing with a lot of parts and want to make parametric notes but want an easy way to find all the ID numbers attached to show the parametric value of each individual part.

For example:

&PTC_MATERIAL_NAME:300 would be one material of a part and &PTC_MATERIAL_NAME:301 would be another. Is there an easy way to find all those identifier numbers at once?

[MartinHanak]

Hi,

I guess your drawing contains assembly as drawing model. How about using a repeat region.

[al3]

Martin,

This drawing is for a bunch of oring sizes that are all different formed shapes, so they will not be an assembly

[MartinHanak]

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@al3 wrote:

Martin,

This drawing is for a bunch of oring sizes that are all different formed shapes, so they will not be an assembly

---

Hi,

If I were you, I'd create an auxiliary assembly that contains all oring sizes. If you have hundreds of such parts, then note that it is possible to automate the assembly of these parts (e.g. by generating a trail file).

[al3]

Martin,

Everything in the drawing for the program has to be released and procured, which an assembly of orings could not. If it's just being used as a drawing aid I cannot go down that approach. I think my best option that I've found is to make a table in excel with &partnumber:200 and then go to some aribitary number like &partnumber:400 and then see which ones populate in the creo drawing when I import that table. I can then take that table and export the table and then see which number corresponds to the part in the creo drawing.

[MartinHanak]

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@al3 wrote:

Martin,

Everything in the drawing for the program has to be released and procured, which an assembly of orings could not. If it's just being used as a drawing aid I cannot go down that approach. I think my best option that I've found is to make a table in excel with &partnumber:200 and then go to some aribitary number like &partnumber:400 and then see which ones populate in the creo drawing when I import that table. I can then take that table and export the table and then see which number corresponds to the part in the creo drawing.

---

Hi,

did you test mentioned solution ? It seems to me that it does not work. If you add note containing &partnumber then it displays parameter value from current drawing model. If you need to display &partnumber related to another drawing model, you have to activate it and then place a note. No ID is used to display parameter value.

[al3]

Martin,

Once I add all the parts to the drawing I can import a table from excel that has something like this

&partnumber:2

&partnumber:3

&partnumber:4

and so on to a huge number

Once I insert this table if one of those ID numbers is in the drawing it will show the parameter associated to partnumber, and if it doesnt exist it will stay at &partnumber:xx. I just wanted to see if there was an easier way to find these without this trick.

Thanks

[MartinHanak]

---

@al3 wrote:

Martin,

Once I add all the parts to the drawing I can import a table from excel that has something like this

&partnumber:2

&partnumber:3

&partnumber:4

and so on to a huge number

Once I insert this table if one of those ID numbers is in the drawing it will show the parameter associated to partnumber, and if it doesnt exist it will stay at &partnumber:xx. I just wanted to see if there was an easier way to find these without this trick.

Thanks

---

Hi,

finally I was able to reproduce your solution. If I remember it well Creo assigns even ID numbers to parts, therefore you can skip odd numbers. Also I agree with @StephenW ... restart Creo and open your drawing before you add your note.

&partnumber:0
&partnumber:2
&partnumber:4
...

[StephenW · Accepted solution]

This usually works well. It works the best if you start with a new session of creo and only open the drawing. Session numbers in a creo session that has opened a lot of files can get really big. I start with zero. I use model_name since it is a system parameter instead.

&model_name:0
&model_name:1
&model_name:2
&model_name:3
&model_name:4

[al3]

StephenW,

This is how I have done it and wanted to see if there was another way, I'll mark your answer as the solution so others with the same question can find this.

Thanks,

Alex 

[pausob]

Apparently, the ability to shown Session ID in the model tree has been implemented in Creo 9.

See Enable Show/Hide Session ID in Model Tree 

Too bad for those who haven't upgraded yet...