Meaty Sweeps. You can gnaw on them all day like a charred piece of sandy camel leather. (Your computer can too.) But what are you to do when you want to send a profile merrily down a path in two directions? at once? in SolidWorks?! Well, can’t be done. BUT, you can use a single set of sketches and a couple features to get that sweep going the direction you want. You can even add in dimension driven constraints! Yes, imagine it for a moment. Take it all in. Then hit the jump to download the file and see how it’s all done.
SolidWorks Mid-plane Sweep
It’s indescribable how many ways you can sweep a profile. Well, it is describable, but it’s a feature with a lot of options that’s simply good to be familiar with. We’ve shown you how to create 3D non-planer Sweeps and how to create just about any kind of Spiral Sweep. Now, it’s time to get a little more control over the flowing feature. First, here’s the sample file for you to have a look at. I did this with surfaces, but it works just as well for solids.
Note: For those that already know how to use the Selection Manager, you can skip down to step 6. Remember though, this Sweep cannot currently be created using one feature, so you’ll be selecting the Profile and Path for two different Sweep features.
- Create your Profile sketch and Path sketch.
- Create a Sweep feature. When selecting the Profile and Path, Right mouse button (RMB) in the graphics area and select Selection Manager
- Use the Selection Manager to select the Profile and Path sketches
- After confirming the selection, you’ll see the sweep generated. Confirm and Exit the Sweep.
- Start a new Sweep feature. Follow the same step above to select the Profile and the Path to use in the Sweep.
- Now, before exiting the sweep, RMB in the Path selection box in the Sweep Properties and select Edit Selection.
- This will put you back into Selection mode, and you will see two selection nodes appear at the ends of the path.
- Grab the Selection node and drag it to the opposite end of the Sweep section you created earlier. Confirm and Exit the Sweep.
- You now have a complete Sweep that extends in both directions from a single Profile sketch.
Now, we could have modifies the boundary of the sweep in that step, but to get the sweep to continue in the opposite direction, it requires another step. Don’t worry though. You can use the same Profile and Path sketches you’ve already created.
Extra SolidWorks Sweep Tip!
You can add extra points or spline points to your path sketch to constrain (or snap) the Selection nodes to. Adding dimensions to these points can give you better control over the boundary of the Sweep.