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Creo 'Save a Copy' Best Practice

N

NKollmar

New member
I have a feeling I'm not using the best practice here...

Occasionally I will save a copy of a drawing and then insert another model into it to create a multi-part print. But if I delete one of the views within the copy the changes are reflected in the original drawing and the dimensions will disappear.

I then tried changing the config option "create_drawing_dim_only" to yes. Now I get the message "when creating drawing dims only, model baselines may not be used" when trying to make ordinate dimensions. This makes sense but I really like to use the "model annotations" dimensions as they seem more stable so I may switch that config option back to no

Is there a best practice? I do copy drawings occasionally and don't want to have to redo all the dimensions in the original drawing every time something is changed in the copied drawing.

Thanks
Nolan
 
When you click save a copy it doesn't work like microsoft office. In office when you click save a copy and save it, you are automatically put into the "copy". When you click save a copy in creo it saves a copy and keeps you in the original drawing, NOT the copied drawing. After you click save a copy -> save, close out the current window and re-open the copy and your problems should go away.
 
I just open windows explorer and making a copy of the file. I work alone and don't have to deal with any corporate file control system.
 
What is happening is that when you delete the sheet or view from the second drawing, it deletes the dimensions from the model and creates a new model (increments the number). To get your dimensions back on the first drawing, first thing after deleting that sheet or view from the second drawing and saving, go into windows explorer and delete the new part models that creo has created. Close your files, erase from session, and re-open, your dimensions will now be back in the first drawing.
 
Silverado8405 - I'm aware of how Creo maintains focus on the existing drawing and doesn't open the new copy. All modifications are done to the new copied drawing and effect the old drawing.

Dr Gallup - I haven't used rename in session before, I'll give it a try.

moldman - Will a physically copied file not have this behavior? I've got some lockdown but could probably get away with this if it would work easily.

dross - Thanks for the explanation of what is happening, that sounds complicated. Does that mean a model can only exist in one drawing at a time as any modifications will erase the others?

Thanks!
 
I typically make three drawings of the same part for different purposes. I have learned to not delete dimensions because that deletes them from the part and then they disappear from the other drawings. I erase them instead. If the dimension only exists on one drawing, you can delete it. It's easier just to erase all unwanted dimensions. If you are going to delete a view, make sure the other drawings are open and then those dimensions will still exist because the view and it's related dimensions still exists in another drawing. This practice of having all the drawings open may solve your problem, but if you only have multiple drawings occasionally, you will have to know somehow that you do. I suspect this problem exists no matter how you make the copies.

I am still on WF3 (thankfully), so I might be all wet in the real world.
 
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OP, the model can be in multiple drawings. As said by moldman, erase any unwanted dims rather than deleting them. However, if you delete a view on a drawing, it will delete the dims from the model unless they are driving dims. That is why you must delete the new models created by Pro.
I've tried as suggested with having all the drawings open, doesn't work for me.
My method does work although it is a pain.
 
dross, how do you create the duplicate drawings. I make copies in windows explorer and manually change the name. It works as I described with all drawings open for me - I tried it before making the post. That method of making the duplicate may have something to do with it. The thought occurred to me that another solution would be to just make multiple sheets in the same drawing, but that would mean creating the desired views again and the desired dimensions. I remember somewhere in the back of my memory that you can merge drawings. I don't remember how to do it, but if remaking the desired views is too much work, you could duplicate the drawing in any one of the above mentioned ways, then merge it to the original and make the desired changes.
 
drgallup,
I just tried the rename in session and did end up with two drawings, but when I removed a view from the newly created drawing it removed all the dimensions from the original drawing view. Maybe I'm not going about it correctly?
 
Look into this config setting

create_drawing_dims_only YES

It's only going to affect newly created dims BTW.

Which brings up the point, why are you creating drawing dimes anyway? You should be showing model dims.
 
I was playing with that setting in my original post and didn't like (or didn't fully understand) the results.
As far as drawing dims vs model dims a lot of my older parts were not modeled very well for showing dimensions and I also like to use ordinate dimensions which I'm still learning about.
 
dr_gallup said:
Which brings up the point, why are you creating drawing dimes anyway? You should be showing model dims.
Click to expand...

I can tell you a very good reason for using added dims rather than driving dims.
Suppose you have an assembly with a bunch of parts mated to one another end to end that are exactly 20 feet long total.
If you use driving dims and change the decimal places on the dimensions it causes the dimension to be rounded off. Do this to a few parts and now your assy is no longer exactly 20 feet long, as each part has been either lengthened or shortened by rounding of the dims. This can cause other parts to fail that depend upon this length being exactly 20 feet.
So, I always use created dims rather than showing dims after I got bit in the butt a few times by this.
 
NKollmar said:
drgallup,
I just tried the rename in session and did end up with two drawings, but when I removed a view from the newly created drawing it removed all the dimensions from the original drawing view. Maybe I'm not going about it correctly?
Click to expand...

Did you have both drawings open when you deleted the view? In WF3 I don't have this problem if both drawings are open.
 
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