Solid Edge has two separate functions that combine to do the equivalent job of SW Configurations. I’m just figuring this out, so it seems that other SW users probably haven’t seen this yet either. SW users use configurations in a lot of different ways. We use it to simplify parts, and we use it to make variations of a part. Solid Edge can do all of that, it just does it a little differently, and it uses the Simplified Parts and Family of Parts functions to do it.
Let’s start by seeing some of the details of Family of Parts.
We’ve talked about them here, but I wanted to go through the exercise of actually making a family of parts and putting a couple variations on a drawing. I also want to clear up a few things that I think people who haven’t used Solid Edge might be confused about.
Can you use Family of Parts on Synchronous parts?
You can create dimensions on synchronous or ordered geometry, and drive the dimensions with a table.
If you want to turn features on and off (suppress/unsuppress), you will need to use Ordered features.
Can you use tables to drive FOP?
Yes, in fact, this seems to be the preferred way. It doesn’t look like you can use Excel, but tables are definitely doable. A Family of Parts table looks like this:
This is pretty nice. As far as I can tell, there is no cryptic syntax at play here like in SW Design Tables. You can even place different configurations in different places (notice the Path fields). The FOP table enables you to change dimension values, suppress or unsuppress features, control text based properties, control Live Rules, and any relationships created in the part.
One really cool thing about the FOP table is that as you mouse over values in the table, the values highlight in the graphics window. This just feels worlds beyond SW and Design Tables. Design Tables always feel so fragile and tentative. If you click on the wrong thing or in the wrong place, the whole thing could disappear, or it might screw up your table. Solid Edge just feels a lot more solid in this regard.
Here’s one I don’t quite understand. In addition to the FOP table, you can also access a Variable Table. I’m guessing that the Variable Table is for controlling a bunch of dimensions at one time, and probably intended for use when you’re not using FOP. You can access all the variables on the Variable Table from the FOP table, but the Variable Table has some extra columns, such as Rule, Formula, Range, Expose, Exposed Name, and Comment.
You can rename dimensions listed under the PMI heading in the Pathfinder (FeatureManager). It’s nice to have all the dimensions listed in one place like this. Dimensions that aren’t named get default names like V3406. This is a really nice way of handling things.
Oh. Here’s one that’s even better. You can select from the RMB menu to show Values, Names, or Formulas. Showing formulas shows both names and values. And then of course you can show or hide specific dimensions using the PMI heading in the Pathfinder, with those little checkmarks next to the listed dimension names. I think this is very nice. I’m not sure why people seem to give the impression that SolidWorks configurations are better than this.
The one thing that I think could go either way is that SolidWorks configurations are all in a single part, and FOP makes a set of completely different parts.
Reading the Help on Simplify shows one of the big differences between Solid Edge and SW. You will rarely if ever find a statement in the SW help that tells you what the conceptual goal of something is. For example, under Simplifying Parts, the Solid Edge Help has this to say:
The commands in the Simplify Model environment allow you to reduce the complexity of a part so that it processes more quickly when used in an assembly. The ultimate goal of part simplification is to reduce the total number of surfaces that make up the part.
It’s nice to know that fewer faces on a model will help it to process faster. This is something it took me a while to learn in SW. I don’t get the impression that Solid Edge is trying to hide information from users the way that SW does. I think SW things they are making it simpler by giving the user less information. But they are wrong, they are just confusing people. Anyway, I’m getting a little distracted here. It’s rare enough to find something encouraging in any software Help file.
The Simplify “environment”, I suppose it’s called, is initially a little strange. They advocate using features to block out other features. So to eliminate a fussy detail, you might extrude a block over it. So additional features added under the Simplify heading in the Pathfinder are kind of like a special use configuration in SW. In the image to the right, I deleted the 7 faces of a hexagonal cut in the top of this part instead of suppressing the cutout. I’m not sure this is really the intended workflow, but it demonstrates the use of the Simplify environment.
You can also save a simplified version of a part to an external file. Which ever method you use, simplified versions of parts can be used in assemblies or drawings.
Hmmm. I’m left wishing that the Simplify environment enabled you to use Suppress. Other than that, I’m finding very little use for the Suppress function in Solid Edge.