Multi "Cut to length" parts in Assemblies

Hello All.
I'm new to Pro/E and so far I'm loving it. I'm really starting to get the hang of it but one thing I need help on is handling of "cut to length" parts.

A few examples of what I mean are: ready-rod, unistrut, din rail, panduit, rebar, aluminum extrusions, etc.

Anything that you want controlled in all but one axis - I use 2 inches of x material here, 4 inches of x material here, 2 feet of x material here - all within the same assembly.

I would like the key parameters to be controlled by a family table (width, depth, etc) because some of these come in variations, but I need to insert multiple instances of this part into my assembly, each with a different length.

What is the best way to accomplish this?
I'd still like the ability to change a width/depth feature or dimension on the "parent/generic" part and have that reflected in all of the instances of it.

Thanks and Best Regards,
Jeff

Jeff,
if your parts are only cut to length, you can use a family table.
If they need further modifications, use them as start parts. If your drawings have the same name as your parts and the config.pro option rename_drawings_with_objects is set to both the drawings of your new parts will be created automatically.
ReinhardN
edit: provided your start part has a drawing of the same name


Edited by: ReinhardN

From how I read what your trying to do I think a nested Family Table is in order. For example if you have a series of rods of different diameters and lengths, you create one family table that has the diameters, than in each instance you would make a family table in each instance of the lengths, which can be easily done if you want them in increments by using the patternize option.


What we do is use a relation in the part that sets the name of the part equal to a parameter called part_no that way for family table parts such as this you comment out the relation and than you put in the part number manually and use the parameter in all of the drawing tables instead of the file name.
I can post you more but I think that there are other threads that cover this.

Depending on what version of ProE you are using, you may wantto look at flexible parts. By making a part flexible you can use the same part but have the length different in the assembly. I think this function is only available in Wildfire. You should be able to find this when in an assembly under edit\make flexible.

All,
Thank you for your suggestions. While I am sure I can get the family table approach to work, since I'm dealing with odd lengths (cut to fit) I'm going to try out the Flexible option - I can see the family table for these common parts getting ridiculously long. That sounds like it might the best approach. I'll let you know what I end up using (for the record).

Thanks again

Regards,
Jeff

Jeff,


If you do the Family Table Route I would suggest incorporating the length in the file name of the instance, for example a pipe that is like 2.5 inches long would be name_2500 that way you can avoid duplicates. Military has a good numbering system for standards.


J

I would use family table for the stock lengths then make the component flexible for the assembly. That way the BOM shows the raw material that you need to start with. The only exceptions would be if you could use the scrap cut off one piece as the stock for a little piece somewhere else. Also, BOM balloons don't work for flexible parts.

Raymon, Dr. Gallup,
Thank you for your excellent answers to my challenge. That is exactly what I'm doing now and it's working excellently (to recap:
1. I have created a family table for "common" lengths and formats
2. I insert the closest matching part from the family table, then
3. I use "flexible" to "cut" the part to the exact size. e.g. I turn a 4.5 in. piece into a 4.17 piece.

Your help has been greatly appreciated!

Best Regards,
Jeff

An alternative to using flexible parts would be to do an assembly cut to shorten the part.