Two facts. There’s nothing that will hone your sense more than realizing you could be riddled by shurikens at any moment and… it takes phenomenal ninja skills to reorient geometry in SolidWorks. Ninja skills, or a fair amount of flailing about like a crazed shuriken thrower, which is exactly how I came upon five tips to help you change up geometry orientation, in SolidWorks, that will totally make you look cool to people who care about that.
Changing geometry is actually really easy within some parts, and a trial of a thousand fires with others.
We’ll take the middle road, so as not to become too badly scarred, and show you the steps you need to consider when attempting such dangerous feats of modeling mastery. We’ll start with an innocent looking knob…
Note: This is not about moving parts around in assemblies. That’s easy. This is about moving geometry around in part files. I know, it should be as easy as moving parts around in assemblies, and can be using a certain feature you’ll see below, but adjusting sketches to move geometry (or features) can be a pain. If anything, this will give you a stronger foundation for building parts and make you think about how you’re creating them, which is always a good thing. hi-ya.
A simple Knob
This knob looks simple, but when you suddenly become brave and try to change how it’s oriented, look what happens.
As soon as you try to move a sketch to another plane or adjust a dimension, features go everywhere and you’re left wondering if you saved a copy. The errors you get with a simple part like this are not too bad to correct, but they do make this simple knob a challenge to reorient. First, lets explain why this happens.
Why SolidWorks geometry explodes
SolidWorks parts are made up of features built on top of other features. They all have a starting point. When SolidWorks can’t find that starting point, the geometry gets jacked up… QUICK. The best way to make a part that needs to be relocated in 3D space, is to isolate the starting point and the references. Here’s how.
Launch the Attack
There are basically five things to remember when you want to reorient a part in SolidWorks:
- Focus on the first Feature
The sketch and first feature should control every other feature after it. The first feature starts from a default plane. After you’ve created your first feature, DON’T use the default planes to create any other feature. You want to be able to move the first feature and have everything else move along with it. It seems like features should just follow their intent, but if you have holes or features referencing other default planes, your part will explode. This means you may need to… - Create your own references
If you want features that move with the first feature, you’ll likely need to add reference geometry, like planes or an axis, that moves along with it. I’ll almost always include a set of planes that are created from the first feature and use those to create the rest of my features from.
A plane created from the first feature to control the sketch in the next feature. - Reduce relations
When sketches are moving around, it’s best to reduce relations to a minimum. I still lock down sketches. I just try to avoid vertical and horizontal relations because they become redundant with collinear or perpendicular relations that reorient better. - Don’t dimension to the origin
Many use the origin to build geometry and dimension off of. It’s easy, but if you move a part and a hole is dimensioned off the origin, it won’t move along with the part. This goes back to the first feature. Use a sketch point or vertex to dimension off of and keep that common to each feature you create. - Test as you go
It’s way easier to test out reorienting parts as you go than finishing it and trying to figure out where to start with all the errors. It’s certainly not the most fun way to model, but you quickly get an idea for what relations and dimensions work.
Download Knob.sldprt (SolidWorks 2009)
After all of this, you may still move it and get odd errors or sketches shifting about. It just can’t be helped. In this case, you may want to attack with…
A Simpler approach
There are actually two ways that are much more simple than dealing with sketches.
Use an Assembly Template
The first option you have to reorient a part in SolidWorks is simply to open up an assembly template, plop the part in and orient it the way you need that bit to sit. This is just regular old adding parts to assemblies to show different orientations. In an assembly you’ll can control part orientation through configurations. Just mate it into position in one configuration, then suppress and add some mates to orient it (or a copy of it) into another position. However, if you are trying to reorient a SolidWorks part to import into another program, the part itself needs to be oriented correctly. Many programs I’ve used will only bring in the part in it’s originally orientation.
Use Move/Copy Feature
The other option, a MUCH preferred is Move/Copy (Insert, Features, Move/Copy…) which allows you to completely skip thinking about how anything is modeled and just move or rotate any SolidWorks body where ever you want it to go. Simple, clean and fast. To me, this just gives a calm disregard for how features are created in a sketch-based modeling program.
Argument for Direct Modeling Features
Obviously, the simple approach above is the direction to go in most cases. Going through the steps above, working through sketches and attempting to move features as you modeled them initially is a good argument for better geometry conditions. Should you have to go through all of the sketch manipulation to reorient bodies? Features like fillets reorient perfectly. They don’t use sketches. Imagine if that’s how every features would work. So, we get rid of sketches, which cause most of the problems, or make them work better. It would be a trade-off of course. With the sketches you get a certain amount of adjustment. Without them, you don’t have to deal with them.
Anyway, I hope this helps you get a handle on how to reorient parts. If you have specific questions about this part or one of your own, just hit the comments and we’ll hash it out.
