Item Number (Find Number) and Part Number in Notes

[wfalco]

Seasons Greetings:

I am pretty sure I can NOT put an Item Number (Find Number) in a note. But at the very least I would like to add the "part_number" parameter. In case below that is "MS20995-C32". This should be as easy as:

&asm.mbr.PART-NUMBER MS20995-C32

-----

1. APPLY SAFETY WIRE FN (99) (MS20995-C32) USING DOUBLE TWIST METHOD PER
NASM 33540.

-----

?

Does not work. I am missing some simple syntax I am sure.

Anyone know?

If Item number is possible that would be great to know as well. But I think that's a dead horse?

Happy New Year All!

WayneF

Creo 4.0 m020

[MartinHanak · Accepted solution]

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@wfalco wrote:

Seasons Greetings:

I am pretty sure I can NOT put an Item Number (Find Number) in a note. But at the very least I would like to add the "part_number" parameter. In case below that is "MS20995-C32". This should be as easy as:

&asm.mbr.PART-NUMBER MS20995-C32

-----

1. APPLY SAFETY WIRE FN (99) (MS20995-C32) USING DOUBLE TWIST METHOD PER
NASM 33540.

-----

?

Does not work. I am missing some simple syntax I am sure.

Anyone know?

If Item number is possible that would be great to know as well. But I think that's a dead horse?

Happy New Year All!

WayneF

Creo 4.0 m020

---

Hi,

1.] &asm.mbr.part_number notation is related to repeat region, only

2.] do following test

> create new drawing

> set part containing part_number parameter as drawing model

> create drawing note and put &part_number callout in it

3.] if drawing model is assembly, you have to use &part_number:session_id callout

[wfalco]

Martin,

Happy New Year!

Yes. Session ID works. I am finding ID thru a round about way using Excel. I queried the ID number and it was incorrect. So in Excel I ran column down to like 1200 lines:

part_number:1

part_number:2

part_number:3

etc.

When pasted into Creo - it exposed all ID's. The ones that don't exist, it blows out the & in front of the line.

So - this works. But I have to visually find each one. Which is not too bad.

NOW....I want to make sure I am assuming that the Session ID WILL NEVER CHANGE- CORRECT?

Thanks,

Wayne

[MartinHanak]

---

@wfalco wrote:

Martin,

Happy New Year!

Yes. Session ID works. I am finding ID thru a round about way using Excel. I queried the ID number and it was incorrect. So in Excel I ran column down to like 1200 lines:

part_number:1

part_number:2

part_number:3

etc.

When pasted into Creo - it exposed all ID's. The ones that don't exist, it blows out the & in front of the line.

So - this works. But I have to visually find each one. Which is not too bad.

NOW....I want to make sure I am assuming that the Session ID WILL NEVER CHANGE- CORRECT?

Thanks,

Wayne

---

Hi,

1.] Session ID is dynamic value related to current Creo session.

2.] Once you set up Session ID, you don't have to worry about it anymore ... Creo changes its value automatically if necessary.

[wfalco]

That word "session"throws me a bit. Make me think of something "in session" like "for the current time" or something like that?

My impression is that these ideas are Permanent....Like DNA or whatever. LOL. Right? They are assigned and will always be.

Now....when someone deletes the component...I imagine it just diverts back to &PART_NUMBER:X (actually the & would drop off automatically) in the note.

[MartinHanak]

---

@wfalco wrote:

That word "session"throws me a bit. Make me think of something "in session" like "for the current time" or something like that?

My impression is that these ideas are Permanent....Like DNA or whatever. LOL. Right? They are assigned and will always be.

Now....when someone deletes the component...I imagine it just diverts back to &PART_NUMBER:X (actually the & would drop off automatically) in the note.

---

Hi,

Unfortunately, I do not understand whether you are asking something. I think you can test session ID behaviour by yourself. For example you can create two assembly drawings and then (a) open drawing1+drawing2 and check session IDs -AND- (b) open drawing2+drawing1 and check session IDs.

[wfalco]

basically just want to make sure the ID's always remain the same number forever.

[pausob]

For sake of completeness:

1) You can implement your own (manual) find-numbers that can be called up in your notes.  It involves creating component level parameters and configuring the drawing's BOM baloons and to display those.  Seems quite feasible for assemblies < 100 (?) parts.  More automated options if you use and configure Windchill.

See, for example the links in this thread:

Fix Index, ProProcess find numbers - PTC Community

2) If someone deletes the component, then drawing notes that referenced its parameters will have the "link-code" text (&PART_NUMBER:X) replaced by static text "***" (three asterisks).  Pity the poor soul who has to figure out what that *** used to mean.

[wfalco]

Pausob,

Good stuff. I may not go there with this. I feel I will get some blow back from team. We have almost 200 parts. This is not normally the case for us. I may just bite the bullet and just manually deal with this for now. I appreciate the info.

Wayne

[TomU]

Wayne,

Session numbers are dynamic and unique to that specific session of Creo.  As models are loaded into memory, the next available session number is used.  If the models are closed and erased from session, the next models to be opened will reuse the same session IDs again, starting over from zero.  For this reason, you don't want to hard code session IDs into anything "dumb" like static text files or saved table files.  If session IDs are used in a drawing (note, table, etc.) or in model relations, Creo will automatically update them to refer to the same component, regardless of what the actual session ID may be for that particular session.

I don't think what you're trying to do is possible.  Some things to consider:

• A BOM balloon will automatically refer to one object in the repeat region table.  It can be configured to display other parameters from that same model, including the model's name.
• An unattached note has no way to access information from other models in the assembly.  There is no command or syntax to pass in the name of a model (or find number) and return other information that can be displayed in this same note.

[wfalco]

Tom,

I  see what you mean by they change. However, they still hold their value. For example:

What was part_number:1 showed "123456" parameter. I erased and then was part_number:23 showed "123456" parameter. So numbers changed but the note remains correct. I thought Creo had absolute numbers for things that were stamped as they occur during creation? 

I guess my only advantage in this situation is having part_number parameter names matching. I thought it would be a good thing. But now I'm thinking....maybe not worth all the effort. But, keep in mind, I have a large amount of notes.

I don't quite understand your 2 other options.

Thanks,

Wayne

[MartinHanak]

Just info ....

If you create drawing note attached to component by leader then you can enter following note text

&part_number:att_mdl

Creo then displays parameter value related to selected component.

See https://support.ptc.com/appserver/cs/view/solution.jsp?source=Sitecore Article Viewer&art_lang=en&n=CS133915 

[MartinHanak]

Hi,

it would help if you attached a picture explaining your situation.

[wfalco]

This is all text stuff. It's hard for me to share pics due to the proprietary information.

But this is the best way I would take a picture of it using samples:

I placed on the side of my drawing:

&part_number:1     which will show the part parameter abc123 to reveal that parameter for "part_number"

&part_number:2     which will show the part parameter abc124 to reveal that parameter for "part_number"

&part_number:3     which will show the part parameter abc125 to reveal that parameter for "part_number"

&part_number:4     which will show the part parameter abc126 to reveal that parameter for "part_number"

etc.

So in my note:

1. PN's &part_number:2 and &part_number:4 shall be free of paint.

Is now:

1. PN's abc124 and abc126 shall be free of paint.

As Tom pointed out....if, for example I open 3 other drawings before this one, the :1,:2,:3,:4 Session ID's will change. But, the value does not. It is still pointing to the parts parameter.

So...

They could now be this:

&part_number:27     which will show the part parameter abc123 to reveal that parameter for "part_number"

&part_number:18     which will show the part parameter abc124 to reveal that parameter for "part_number"

&part_number:9     which will show the part parameter abc125 to reveal that parameter for "part_number"

&part_number:7    which will show the part parameter abc126 to reveal that parameter for "part_number"

So your original answer is correct. This works.