Solved: Re: adding the part number to a note

giobar19 · ‎Oct 18, 2023

I'm using Creo 7.

I want to add a note with the part number in a drawing.

I use the following note when I insert the view of a new part in a multi parts drawing:

&PARTNUMBER
SCALA &scale

The &scale refers to the general scale of the view.

I saved the note in the note folder and when I place the first view of a new component I add a note and load the saved text from "Note from file":

In this assembly I added many parts (they are for a welded carpentery):

If I want to change the scale of a component, I have to select the component from the above list, then change the scale, then select and go back again to the main assembly.

But if I place the view and I change the scale in the view options, it allows me to change the scale of the view in a fastest way:

Creo adds a note with the view scale.

I tried to add the part number to this note loading a saved note but it doesn't works.

Only way is to add the text directly, but this is uncomfortable.

I can add a note with an offset from the scale note but the result is not the same for all the notes, so I have to manually move the text and align the better I can:

full note

offset note

I tried to modify the saved note as follow, but without results:

&PARTNUMBER
SCALA &view_scale

Is there away to solve the issue?

Thanks

pausob · ‎Oct 20, 2023

FYI, it won't help save time with old drawings, but you can perhaps adopt this procedure for your new drawings:

First, prepare a file called "standard_standard_view_note.txt" and put it in your Notes directory

the note file will contain the following:

&PARTNUMBER
SCALA &scale_of_view_new_view

1) add model(s) to the drawing

2) activate a model. add a generic view. rename it to new_view, (and use the "default scale for the sheet").

3) after view is created, create a note from file (using standard_standard_view_note.txt above)

4) the note will show the part number and the view scale. relate this note to the new_view

5) rename new_view to something that makes sense (e.g. name of the component in question). You will see that the created note will automatically be changed

6) repeat steps 2-5 for the other views / components.

Now your view notes will automatically update if you change the scale of the activated model.

They will also update correctly if you change the view to use "custom" scale (system will also create that special view scale note - but you can just delete it).

Little bit of up-front work but should help when scale modifications need to be made - and naming your views is a good idea anyway 🙂

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KenFarley · ‎Oct 18, 2023

I think I understand what you are trying to do, but I'll explain what I think, too.

It seems you want to add to the text that tells you the "custom" scale for a view. You want the added line to be the part number for that view. I do this a lot when I'm using multiple models in the same drawing, to show different versions or that kind of thing.

If you are using a parameter called PARTNUMBER for the information you want to add, you kind of had the right idea. The "trick" is that in a drawing, if I type &PARTNUMBER into a note, it will display the value of that parameter for the model that is currently active. In order to have it show the PARTNUMBER of the model you want, you have to make that model active first.

If you have more than one model in the drawing and you type &PARTNUMBER into a note, you'll notice that Creo will add the SessionID for the active model to the parameter name, so it will say something like &PARTNUMBER:12 or something like that. That's normal stuff and helps Creo to remember which model is being referenced in the note text.

I've used this type of thing in standard notes, detail view labels, and any other Creo-generated or manually generated text. It's nice because it updates if I change the parameters being used, and is especially good if I copy a whole design and change all the part numbers, descriptions, etc.

giobar19 · ‎Oct 19, 2023

Thanks Ken,

I'm using this feature for years, so as you said, when I add a new model view, I immediately add the note to link it to the correct Session ID.

What I'm trying to do is an evolution of what I did up to now to faster the modification of the scale in multiple parts drawings. It happens many times that you place multiple parts on a drawing and at ab certain point you figure out that you have a lot of unused space, or you need more space to add other parts. If I have to modify just one component this is not a problem, but when you need to modify the scale of 15-20 components, then instead of 10 minutes I waste just 2 minutes.

I would like to use the "note from file" on the custom view scale note to avoid to make "copy and paste" the &PARTNUMBER from an external text file.

Another solution could be to modify the standard Creo generated note for the custom view scale adding the &PARTNUMBER, so when I use a custom scale Creo automatically add the part number and the scale.

Thanks,

Giovanni

KenFarley · ‎Oct 19, 2023

Ah, I have had the same problem. Drawing with multiple models and I want the scale for all views to change. I've never found an easy way to do it. I thought it might be possible to use relations, but for reasons I don't remember it didn't seem to work out so well for me. I still have to "visit" every model in the drawing and set its scale individually. Not fun.

pausob · ‎Oct 20, 2023