Avoiding redundant drawing effort

[wrs23]

Our design engineers create part models and then a drawing file to reflect the model. Then as a manufacturing engineer, Icreate an inspection document showing operators the process for inspection. I've been instructed to add a sheet to the drawing and then generate the views and the dimensional characteristics from scratch. The issue is that most of the information I need to generate is already done with the model print - (I.E. our inspection instructions are basically streamlined blueprints). I feel like it would be much faster to remove the few unnessesary elements than to regenerate and configure all the views, dimension, etc.


The engineer that developed this process says that I can't use the existing drawing because:


ProE won't allow double dimensioning across drawing sheets


Saving the drawing as something else is still referenced to the part so it is a security risk to have other users possibly destroying the model


It's much better to organize our inspection documents within ProE drawings as additional sheets


The better I get at ProE, the less time it will will take to regenerate the necessary items (I'm pretty darn quick though already)


Anyinsight you can provide would be great -


Thanks

 

[vlad1979]

ProE won't allow double dimensioning across drawing sheets

You can create as many dimensions as you like on top of the others.


If you get the dimensions from the model with show/erase then you can show only the dimensions created in model. In model you can create only one set of dimensions but you can put the same dimensions a hundred times with .ref


But if you create the dimensions in drawing, which I think is best in your case (not to change the model) then you can add as many dimensions as you like.

 

[vlad1979]

just had an idea, don't know if it works but give it a try.


For you not to create againall the views and dimensions on the second sheet, there could be a way to copy the entire sheet on the second one.


Save a copy of the current drawing. Name it whatever, say "X". Then in the first drawing go to insert / shared data/ from file and select the drawing "x". And a new sheet should be added with the same views and dimensions. Then delete the "x" drawing file.


Now, if I think better the dimensions on the first or second sheet could dissapear because I don't think the same dimension &ad43 or &d52can be shown on 2 sheets at the same time.


But anyway give it a try, see what happens, I'm curious, but at least you could end up with all theviews and notes, you will have to create just the dimensions.
Edited by: vlad1979

 

[dross]

I wouldn'r create a second sheet, I'd either add necessary dims with inspecttion ovals and/or add inspection ovals to existing dims to define which dims need to be inspected.


Added dims would be ad's, not d's.

 

[dr_gallup]

When we need process sheets to show a particular machining operation I do one of two things. Both involve "proper" model creation methodology so you may not be able to incorporate it into existing models.

For relatively simple machined parts I use family tables and create the features in the order they are machined. Sometimes it is necessary to group features to make a manufacturing operation. Then add the features or groups to the family table. Now add the part instance model(s) to additional drawing sheet(s). You can now show the dimensions again because they belong to a different model.

The second technique involves more complex parts where there might be one forging or casting that produces multiple parts. Use either assembly merge or inheritance techniques to get the raw geometry into your finished part then make your machining cuts. You can have multiple steps (merges) if your manufacturing process is complex.

You can also combine the two processes with a family of castings and a family of finished parts where one of the variables in the finished part table is which casting you start with. Lots of ways to skin the cat.