I created this object with a dovetail joint in the middle and then realized it may not fit together after 3D printing unless I put some spacing between the objects. What might be the best way to go about this? And what might be an appropriate amount of space in this situation? attached is a screenshot and shapr file.
You can do this in a sketch by using the offset edge tool in the sketch and then trim the excess lines in the gap to form closed loops on each side of the joint.
You can also do this on the bodies by multi-selecting the faces of the joint and using the offset face tool. Multi-selecting the faces on both sides can be done by hiding one body, selecting the faces of the other, hiding that body and showing the hidden when, and continuing the multi-select of the visible body’s joint faces.
Doing this with the bodies instead of the sketch will allow you to adjust the Face Offset : Offset Distance in the history so I’d prefer that.
As for the spacing, it will depend on your material, 3d printer, etc. You probably need to isolate the joint (print a sufficient amount of the part on each side of the joint) and test it before printing the whole part. If it’s just a one off, sanding may be your friend.
It really depends on your printer and the filament you’re using. For example, with my printer, I use a 0.1 mm gap (0.05 mm on each side) if I want the joint to fit together freely.
But since my printer is precise enough, I wouldn’t apply any gap for this particular project — in this case, the joint will fit with a bit of force but will hold the parts together securely.
I think the best way in this case will be face offset as @shaprvision said.
Just for your information — a sketch can be controlled using variables, so the gap can be designed and adjusted at any time.
Yes, variables can be used in the sketch but not with offset edge as far as I know. You’d have to draw both sides of the gap and then constrain it using one or more variables. Even then, the variables must have positive values (0 is not allowed).
With Face Offset, the Offset Distance allows for 0 and negative values. This can be beneficial when printing parts since material can shrink and he may find that 0 gap in the model yields a suitable positive gap on the physical parts. You could also assign a variable to the Offset Distance of multiple Face Offsets (e.g. if you have multiple similar parts that modeled and require the same gap) if you wanted to centralize the value in one place.
For sketch variables since we don’t have offset constraint (missing feature) no need for negative values.
Correct. But you can use offset and then constraint it
Variables can have negative of zero values without any problem. But distance between (say lines) cant be negative (but can be zero).
I’m not against offset face, more than that I suggest to use it in this particular case (in message above).
That’s not the best idea to control shrinkage in the CAD. Much better compensate this in slicer before print and for every filament separately.
What stop you from using same variable everywhere you need it? You can even use it in offset face and in as many sketches as you need same time 
Conclusion: The advantages of each method should be evaluated on a case-by-case basis. Claiming that one approach is always better than the other is fundamentally incorrect.
Variables can have negative of zero values without any problem. But distance between (say lines) cant be negative (but can be zero).
Of course but in the context of this they can’t.
That’s not the best idea to control shrinkage in the CAD. Much better compensate this in slicer before print and for every filament separately.
Possibly but again, in the context of the question where he’s trying to model the gap, the flexibility of using 0 or negative values (and the general limitation of using a variable) was the intent of pointing this out.
What stop you from using same variable everywhere you need it? You can even use it in offset face and in as many sketches as you need same time
Agreed. I was just mentioning the use of a variable in multiple Offset Faces b/c it sounded like we were arguing between that and variables.
Conclusion: The advantages of each method should be evaluated on a case-by-case basis. Claiming that one approach is always better than the other is fundamentally incorrect.
Agreed. I wasn’t claiming one approach is always better. I was just providing information about each method to help the op as I think you were as well.
Hi Mark,
Good info above! I would add that it is often useful to make a small test to get some real data where you can see/touch the result without printing the bigger piece. So I’d use your design and split it twice to yield 2 pieces; just the dovetail. Then print a trial, evaluate, change the variable of face offset (or however you choose) and repeat until you’re happy. Finally suppress the steps in history used to make the testers.
Once I got my head around the idea of multi-selecting the faces of a joint and changing the values, it seems the most straightforward way to go. Am tinkering with it now.
Hmmm, it never occurred to me to try it with no gap! Am printing a test now to see if the pieces with go together without a gap.
Good advice! I split the pieces in my splicer (Bambu Studio). They are printing now. We’ll see how it turns out.
Thanks so much for the helpful discussion, which I will save in my Tips and Troubleshooting folder! Alas, it turned out that I needed no gap after all! I would have never imagined it. After printing a test, the pieces fit together quite nicely. Attached are 2 images, one with the pieces flush with each other. I did learn some ways to create a gap!
Again, thanks so much!!!
Mark
