Seeing which constraints are on a sketch
hey @happyday.mjohnson,
The distance constraint is called a dimension in Fusion 360. You can get to this via the sketch drop down or hitting D on your keyboard. Once the sketch dimension tool is active you can select two sketch entities which will create a dimension.
When you say distance constraint, do you mean dimensions in a sketch (I assumed it was, but want to be sure)? If so, here is my understanding of your question -
1. You have a sketch to which you have applied a combination of geometric constraints (such as collinear or parallel or symmetric, etc) and sketch dimensions.
2. You are continuing to add sketch dimensions and the overconstrained dialog pops up.
3. You are trying to figure out what is preventing you from adding that dimension.
Is that correct?
Best Regards,
Unfortunately there is no easy way to determine what is causing the overconstrained situation. If you are willing to share a link to your file along with details of what dimensions or geometric constraints you are trying to add, I'd be happy to take a look and see if I can help you figure out options for geometric constraints/dimensions that may need to be removed for it to work.
Here are a few tips that may come in handy as you work with sketches. None of these will help with automatic identification of why the sketch is overconstrained or what else needs to be added to get it to be fully constrained, but hopefully it helps with methods to analyze those situations.
TIP 1:
1. Launch the Preferences dialog (access it from your username drop down in the top right of the UI) and click on the Preview option in the left pane of that dialog.
2. Check the box "Sketch - color sketch geometry based on constraint status".
This will give you visual cues as you are constraining your sketch entities. If you didn't want an entity to become fully constrained because you were going to add, say a dimension to it later on, you will see it become constrained immediately (as its color will change), so you can choose to leave it unconstrained for the moment.
TIP 2:
1. Capture your design intent as you develop your sketch. That is, if you want entities to be related geometrically (collinear or symmetric, etc) add those first. If the location of entities relative to one another are more important, then add those dimensions before adding geometric constraints. (That said, it is generally preferrable to add your geometric constraints first).
TIP 3:
1. Set your selection filter to only "Sketch Geometry Constraint".
2. Window select everything in your sketch.
3. Right click and select "Toggle Driven".
4. This will convert all your sketch dimensions to "Driven" dimensions.
5. Now, methodically add the dimensions that you need.
6. When done, you can right click on the dimensions you toggled to Driven and try changing them back to Driving. If you encounter the overconstrained message when setting them back to Driving, you can look at the dimensions you added for that entity and decide which ones to keep.
TIP 4:
1. When you try to add a constraint (either geometric or dimension) and you get an over-constrained message, try grabbing the sketch entity to which you were trying to apply the constraint and moving it.
2. If it doesn't budge, also try moving its end-points to make sure it is fully constrained.
3. You may have to repeat this on all sketch entities that are related to the one you are trying to constrain.
4. If the sketch entities cannot be moved, then your sketch is fully constrained.
5. At that point, if you still need to add another constraint (or constraints) that is important for you to capture, you can remove one or more of the existing ones, repeat the above steps to make sure it is no longer fully constrained and then add the new ones.
I know the above doesn't help you get past your immediate problem, but hopefully helps with future work. As I mentioned if you are willing to share your design, I'm happy to take a look.
Best Regards,
