When I switched to Solid Edge as my main program for SLDD, I ran into one small problem---part families; I did not know how to do them in Solid Edge. Part families are parts that share similar characteristics, but certain geometries may change (like length of a bolt). All of that data can be stored in one part. In a world where Solid Works is king when it comes to configurations (SolidWorks' lingo for part families), I had to figure out how Solid Edge performed a task that SolidWorks does effortlessly. I want to pass on what I learned though the process to you. It was actually quite easy.
As above, the easiest example I can think of for the way a family of parts works is the good ol' standard threaded screw. There is no need to create a separate part file for every single length bolt for say a 1/4-20 bolt. We can actually handle that in once single file in Solid Edge; however UNLIKE SolidWorks, in order to use that bolt in an assembly, it must be populated out into it's own file once the data is created. Read more to find out what I mean.
Disclaimer: This is my system for Family of Parts. if you have a better system, please let me know. Also, this is not a beginners how-to. You must have a firm grasp of how Solid Edge performs as I cannot put every detail into these instructions.
There will be a little bit of a setup when it comes to using the Family of Parts system in Solid Edge. As mentioned; yes all of the data for changing variations is handled in one file in what we will call the "master" file. But once the variations have been setup, we HAVE to populate the members out. The first issue you will run into is when populating, the populated files will be saved to where the "master" file is located. So what I found works best is to set up a folder for each part inside a master parts directory. Within that folder will be anything related to that part such as the Master part file, the family members, and the drawing related to that part.
Above you can see my typical setup for my library of parts. As you can see, there are only folders listed. This makes for a clean setup and makes parts easier to find. In my Solid Works Directory, it is smorgasbord of parts, assemblies, and drawings all dumped into one folder. With this setup, only files that pertain to THAT part are in there. This also ensures that Family of Parts Members are populated from the Master file into the correct folder--as long as that master part file is in its correct folder.
Above is an example of a 10-32 screw parts folder. Here you see the "Master" file that I keep referring to (I'll get to this shortly). You also see the drawing file (.dft file) for the part. Lastly, you also see the "populated" family members. This is my standard setup for EVERY part that I create. In this instance, the dash numbers do have a meaning, they represent the screw length in 1/16th increments; your part numbers or dashed number can be whatever they need to be.
Now that you have the folders setup, you can create your part. Just open up a new part file, and model as you normally would; Extrude, Cut, Revolve as your heart desires. Now this is only for this example as my screw lengths change, the length dimension is my changing variable that makes up my "Family of Parts". Soooooo.....when I modeled it, I made sure that I gave that dimension a name (double click on said dimension and rename)
Once done Modeling, you can start to create your Family of Parts by clicking on the "NEW" icon (shown in red) on the Family of Parts menu as shown below:
Once you have your part members named (you don't have to do this all at once), then its time to change the variable(s) that sets them apart. It may be a length change as in my screw example, or it may be suppressing certain features.
If it is a dimensional change like mine, simply click on the Variable Table button in the above picture circled in blue. Once clicked, you will get this table:
If you look carefully, you will see how my "LENGTH" variable changes. You simply click in the box like a Excel table, and change to desired size. Once you click "Ok", proceed to save the part. I HIGHLY recommend you attach the word "master" to your part as I have done with my master part. You now have created your "MASTER" file.
Now to cover the other base of it not being a dimensional change. Let's say you have a part where certain features are suppressed. The easiest way to handle this is yet through the variable table shown below. Simply click on the empty box to the right of the feature, underneath the said part and either click "Suppress" or "Unsuppress". Keep in mind that ANY other feature that uses that feature as a "parent" will be affected and will need to be suppressed as well. You will know immediately of this once you look at your feature tree and see grey arrows or red exclamation points beside the features.
The other method to changing suppressed variables is to do so on the Family of Parts menu. You need to have the said family member active on the Family of Parts menu (highlighted in blue). Then click on the feature in your Feature Tree. Then on the Family of Parts menu, click on the suppress icon (highlighted in red). Again, you will need to do this for any children features as well. Using this method only suppresses it for the active family member.
Now the last part of creating a Family of Parts database---Populating. You see, this file does NO good to bring those various family members into an assembly; they have to be populated out to use. Now to do this; its pretty simple, click on the Variable Table on the Family of Parts Menu as we done previously.
There will be a series of buttons located at the top, we are interested in the group circled in red. Of those three, we are interested the the two above. Simply click on Select All Members and then click "Populate". Depending on the part and the amount of members, it could take second up to a few minutes to populate. Once done, you will see the "Chainlink" icons like you see on mine above. This indicates that the part has been successfully populated. If you ever see a clock icon, simply click on the member and repopulate. This usually happens when the part geometry has changed. You can also click on individual part members and populate them as well; you don't always have to click "Select All Members."
You have successfully created a Family of Parts in Solid Edge! You will now see a list like this in the part folder:
I should note that for assembly and drawing purposes, NEVER use the "MASTER" file as the reference; always use the needed family member.
The caveat now to this system is when changes are needed, you make them to the Master part file. The family members are mere part copies. Sure you could cut and extrude on the family member parts files, but it is not wise practice; always make changes to the Master file and repopulate.
As you can see, when a family member is opened, there is no build history. You can open the master by right clicking on the "Part Copy" icon though.
Stay tuned for next week when I cover Family of Assemblies in Solid Edge. This concept goes hand in hand with Family of Parts, but behaves slightly different.
If you have any questions regarding this system, please feel free to email me at firstname.lastname@example.org