They’re a little bit easier to handle than the teething undead, but all the relations in a SolidWorks sketch can make modeling, and specifically concept modeling, a relation re-defining nightmare that is way less interesting than cleaning up after a zombie child.
One of the biggest problems you’ll have with relations automatically added to your sketches is the ‘ON EDGE’ relation created when you use Convert Entities. It’s quick to add them, but takes time to fix’em.
They are the ideal tool for quickly getting the edges off one part into another sketch, but you’ll feel some pain if a change occurs that affects them. Here’s all the reasons to avoid the On Edge relation, what to use instead and tips for when you do need them.
Why relations suck and also don’t suck so much
One thing that really sucks about fending off the scary creatures of sketch-driven modeling is all the intermingling relations you add to create each extrusion, cut, sweep or surface. If one referenced face or edge is deleted or redefined, your model is open to a beastly attack of errors and time-consuming re-work.
It sucks because you have to go in and out of sketches to fix broken relations and it tends to feel like opening your hood to start your car. If we have to use sketches I’d think many would prefer the ability to edit them without going into the sketch, but for now, we need to and one of the most common relations you’ll be fixin’ is an ‘On Edge’ relations created with the Convert Entities command.
Relations are nice because you can quickly make changes to the sketch that completely change the form of the object. They add a bit of structure to the process of creating geometry, and who doesn’t need a bit of structure in their life.
Really, relations are the battle of good vs. evil no matter which valiant modeling decision you make. It’s rare I have a sketch that does not get redefined at some point or another. That means, it’s rare that I don’t have to mess with relations or get rid of On Edge relations, so let’s get rid of them. Here’s what to do.
Don’t Use Convert Entities
It’s one big conflicting feature. It makes creating sketches quick, but can add a lot of headaches to how sketches are handled in context of the edges they are referencing. Did that sound like a mouthful? It is. Convert Entities is a sketch tool that allows you to quickly convert the edges of solids into sketches to extrude. It creates an ‘On Edge’ relation. One simple relation for one simple edge, or so it seems.
Using Convert Entities creates less relations, but more external references
Not using Convert Entities creates more relations, but less external references
It’s when you start converting multiple edges and going through multiple design iterations that all the converted edges can cause errors to appear in your sketches. It’s not that Convert Entities feature is bad in itself, but a lot of the relations created using Convert Entities can go dangling (loose their reference) if some geometry up in that history or features changes. Yeah, it can happen anyway with any kind of relations, but if you reduce the On Edge relations used, you reduce the amount of rework to your sketches. This is particularly true with external relations.
But the biggest reason not to use Convert Entities? On Edge relations takes longer to rebuild.
Reduce the Rework
(Boy, this post is getting longer than I expected.) Here’s an error you’ll commonly get when using Convert Entities.
It happens when trying to delete On Edge relations that conflict with each other. You will typically have to delete every On Edge relation and re-work the sketch to lock it down.
Instead, here’s some tips to reduce rework and rebuild times for your models.
- Use rectangle sketch tool
The simple example. Instead of converting entities on a face that would give you four On Edge relations, sketch a rectangle, attaching the two points you pick to the other geometry.
- Set up shortcuts for relations
adding relations instead of using Convert Entities does take longer, so use your keyboard to make adding them faster. I suggest setting up the most common, Coincident, Concentric, Colinear, and Coradial.
- Re-relate before you Delete
This goes for any sketch entity. Before you delete it, look at the relations (Tools, Relations, Display, Delete…) and remove any that are causing conflicts. Then rerelate them with those keyboard shortcuts you set up.
- Show others how
Show others how to use relations. Some people just don’t know about how they work or what they are for. A feature using a fully-defined sketch will also rebuild faster.
When you do need to use Convert Entities
Here’s some tips for when you do need to use Convert Entities.
- Select Tangency/Loop/Chain
Instead of picking and converting each edge, right-click on an edge and choose ‘Select Tangency’ or ‘Select Loop’ (or ‘Select Chain’ if you’re selecting sketch lines.) This allows you to quickly select a group of edges without the tedious picking about.
- Mark an Edge
This isn’t an option, but can aid in making changes. When you select an edge (or face), convert the edges to sketch lines, extrude and then add other segments to the sketch it (should) update with the changes. Add a point to the line you picked to convert.
- Don’t Use Parallel and Perpendicular Relations
These are usually redundant relations that can cause conflict, avoid them if at all possible. Same goes for the Intersection and Fix relations.
- Use Parallel and Perpendicular Relations
When creating Library Features and want them to work, use parallel,perpendicular and symmetric relations instead of any others. This will help them work in any orientation.
Relations can be a big help, but they are one of the basic features in SolidWorks that are not always appreciated and understood. I’d like for relations to be more geometry related than sketch related in some cases, but that gets into a whole other argument.
What are your hang-ups about relations? Any other tips?