How to create parts that change only a dimension? 1

[battassini]

Hi,
I`m a ProEngineer user, and I`m beggining to use SE. I know ProE has a feature called "family table" that allow users to create parts based on modified dimensions. Is there any similar feature in SE? How to use that? I would like to know any directions... Thanks!

 

[Kenny_G]

Solid Edge has similar functionality, but it is called Family of Parts. On the part that you want to create a family for, select the third tab to the right on your edgebar (Family of Parts). Create your family memebers and then select the dimension you want to control either by dynamically editing the feature or using variable table and add it to the variable section by clicking the Add button. Then change the variable to the proper value for each member. You can also select features for each member to supress if needed. When complete, select the Populate Members button which will save each member out to it own file which will be associatively linked to the master file (the one where the members are defined). Do not use the master file for anything such as drawing views or in assemblies.

 

[battassini]

Thankyou PellaKen!
I've done it now, and I understood. Now you started another question for me: Can I make a drawing with a table of "instances"? I would like to create a drawing generic, with a dimension with the symbol "A" and a table with the three parts and the value "A" for each one. I'm thinking to use Excel, but it seams to be a question more complicate than my first one...

Thankyou again!

 

[roblom]

Under 'Variables' of the 'Tools' menu you see al your dimensions. You can connect the values to another value. If you're in the assy envoirement, choose 'Peer variables' instead of 'variables' and click the part you want to make master copy the value (right mouse button). Click on the part you want to make driven sselect the value and paste.

 

[Kenny_G]

Battassini,
You cannot create a tabulated drawing automatically from a family of parts file, but you can build it manually.

Make sure that you never use the Master FOP file for drawings or assemblies as it is dynamic based on which memeber was applied when it was saved. Instead place the members in assemblies and drawings.

To create a dimension with an Alpha character, switch the Dimension Type (second button from the end on the dimension ribbon bar) to "None". Then set the Prefix option to the Alpha character you want (I usually include a space or two in from to center it in between the dimension lines).

The chart can either be drawn by hand or placed using Excel.

Ken

 

[fwc]

There is an Excel file with macro program might interest you.
It's located in computer directory C:\Program Files\Solid Edge Vxx\Custom\Bearing (the location depends on where SE is installed).