Is it possible to drive the length of a cylinder of a certain diameter from the volume of another part? I'm thinking about using an equation but how do I get the volume from a different model? That model is also split and I want it's total combined volume. I want the total volume of SPF1753-HS1 to drive the length of SPF1753-CO. See attached.
Message was edited by: Scott Giffin
I appreciate the response Matt. I posted my parts but still haven't had a kind soul come up with a solution yet. I understand the addition of the external part name in the custom property as you mentioned but am still at a loss as to what the format of the formula would be to drive the length of my cylinder from the other models total volume. I really didn't think this one was going to be that tough to figure out. I greatly appreciate anyone helping me out with this one if you know how it's done. Thanks!
You uploaded 1 of your parts. You need an assembly and the other part. I think one reason that you aren't getting responses is that what you are trying to do is strange.
Here's one way to do what you want.
Create an assembly with your two parts. Create a global variable with and assign it SW-Volume in your "driving" part:
Edit the part you want to "drive" and double click on the dimension you want to assign the volume to and in the feature tree click on the Vol from the driving part:
Always remember to keep the "driving" component above the "driven" feature in the feature tree. Otherwise you can create what is called a circular rebuild and that should be avoided. And as I said before, this would be better handled with a Master Part driving both of your components. I just took a shortcut to show you how this could be done.
Thanks Matt! I'll give this a shot as soon as I get a chance. I thought I uploaded 2 parts. The length of one to be driven by the volume of the other. I'll have to go back and take a look at what happened to the other one. As far as this being strange... I can't believe more cold forming design engineers aren't requesting this. It's such a basic thing we use every day. You draw the model of the finished part and use that volume to calculate the progressive parts for each preceding forming sequence all the way back to the length of the blank you cut off the wire. While the calculations are easy, I like automating things as much as possible. Thanks again for your time Matt. I really appreciate it!
I see now why you thought this request was a strange one. Now that I've had time to look at the solution you posted I can see that I wasn't clear enough explaining what I wanted to do. What I'm trying to do is use the volume of my finished part to drive the length of each of my previous 4 stations parts so that their volumes remain constant. Each previous station diameter will be smaller than the last but the volumes remain constant. Therefore the lengths will be longer. I want to drive their lengths from the volume of last part.
I'd insert the part inside the part and bring whatever you need to get your dimensions and then delete the body and generate whatever you require.
I was unaware of why when I added a dimension to a custom property it always had the part name appended to the dimension name. It is exactly for a scenario you are describing.
Furthermore, this may be a candidate for a Master Sketch Part type model, where both of your parts are driven by a master part at the top of the feature tree. This Master Sketch Part can contain both the volume and the length, dependent on each other however you need, and then you use that part to drive your two parts. The benefit of doing it this way is that you eliminate a possible circular rebuild problem that you can run into by linking your parts together directly.
I'm sure if you posted your parts or some screenshots, you'd get more targeted help.