How to document mutiple configurations of a part

[DominicG]

Back when we used AutoCad, documenting multiple configurations of a part was easy. You just started a drawing, drew a generic version of the part, added some dims like "A" for length, and "B" for width, set up a table with all the different lengths and you were done.

Now as you all know, with Solid Edge it's more like the "real world". In some case, you create a "Family of parts" and handle the multiple configs that way. However, documenting that in ONE draft file is WAY different now. Having a chart on your drawing now is a much more complicated affair. I'd prefer NOT to have "n" number of drafts (where "n" equals the number of separate configurations) for each configuration.

Call me greedy, but I'd like to have the best of both worlds. I'd like to see ONE drawing/Draft file that features a chart (or parts list) that would automatically update itself when parts were changed, deleted, or added to the family. In short; Can we do this. How can we document multiple configurations of a part in a single Solid Edge Draft? Does anyone have a simple solution?

 

[fredericmenage]

Hi,

There is no really simple solution (especially if you use Family of parts).

The easiest I found was to :
1- make the part adjustable (menu Tools/Adjustable part) by choosing which variables can change.
2- create an asm and insert the adjustable part X times (as many as there are variations)
3- create variables in the variable table of the asm for each dimension of each variation. Expose all these variables.
4- RMB on the parts (one after the other) and choose Edit adjustable part, choose the line, then click on the button to access the var. table (top left)and click on the grey square to the left of the var. you want to link and close the var. table (repeat that same operation as many time as needed)
5- create a dft with a view of this asm. Edit the properties of the view/display : hide all parts but one. Place dimensions and click the grey 'x' to hide the value (top right) and enter a name in the suffix
6- draw a table with callouts inside (you can attach them to a nearby intersection of lines with the leader and then hide the leader. Some of these callouts will be the values from the asm (use property text)

It's not as complicated as it seems but I'm not sure this workflow with adjustable part will always be appropriate...

HTH

Fred

 

[swertel]

Dom,

1) Create your FOP models as you normally would in order to use them in an assembly.
2) Create your draft and choose any one of the members. DO NOT PICK THE MASTER BECAUSE ITS LAST VIEW IS DEPENDANT ON HOW IT WAS LAST SAVED!
3) Dimension.
4) On the dimensions you want to tabulate, select the dimension and click the tolerance button on the Ribbon Bar.
5) Select the greyed-out X to remove the dimension value.
6) Add a prefix/suffix with the correct letter.
7) Create your table manually (Excel or text boxes).

--Scott

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