Scaling object for 3D printing

[lazze]

Hi, I was stuck on a small problem, and I started writing a question. But I found a solution, so it turned into a tip.

I have a sketch that is the basis for a revolved object. The sketch has a parametric offset for the thickness of the shell. This by itself is elementary and works fine. 

But: I now want to be able to scale the sketch down to make a smaller verison of the revolved object, the thickness will then obviously also scale down, which is not good for 3d printing.

My solution was to create a new parameter called "Scale", and then divide all values I want to remain unchanged by the scale by Scale. Parameters for thicknesses and clearances are obvious candidates. This seems to work great.

Any other solutions to this out there?

[SaeedHamza]

Nice way of thinking, but you should have asked if there was something that can save you all this trouble, which there is.

You only need to create the profile you want and then give it an offset, then any changes will keep the thickness as is ... in other words, it's about defining/dimensioning your sketch

Regards

[SaeedHamza]

Here is an example

[laughingcreek]

True, except the offset command in Fusion kinda sucks (lots of bugs associated with it), and you end up with more sketch geometry than you need.  The OP's approach will allow changing the scale to try multiple sizes by just changing a single parameter.  This is a pretty common work flow for small machined parts an for jewelry, where certain dimensions must be maintained, while scaling other aspects of the design.

[SaeedHamza]

@laughingcreek

I'm not sure what issues could come from the offset command

Could you attach something with the case you mentioned?

[lazze]

Thank you for this. My issue arrises when you exit the sketch and revolve the path into an object. If you scale that object, the offset parameter you set in the sketch effectively gets  scaled too. This can result in 3D preprinted walls becoming too thin. Sorry if I didn’t make this clear.

[SaeedHamza]

oh I see, a lot of factors to consider 🙂

Best of luck

[lazze]

I agree. I really would like to avoid using the offset as it gets hard to maintain all those duplicated lines as the sketch grows. I guess the alternative is to model a solid and hollow it out after rotating it to create an object if the geometry is simple enough to allow for this. Which is not the case for my sketch.

[lazze]

I tried making a second sketch and then project the desired lines in there so that I could keep the original sketch clean, and use the second one to create the offset. It quickly became buggy and hard to maintain.

[SaeedHamza · Accepted solution]

@lazze

Did you try to create the revolve in the patch environment as a surface and then scale it then thicken it or use offset face?

or create a solid one and scale it then shell it?

Please let me know

and if you could share a picture of the body you're using for this approach it would be great, I wanna try it

Regards

[lazze]

That is an interesting suggestion. I will try it later or tomorrow and get back to you. It would remove the need for an offset in the sketch.

[lazze]

Sorry for the late reply on your suggestion. Creating a patch and then thickening the patch works really well, and removes a lot of clutter from my sketch. The only downside is that the resulting shape needs a little trimming since it is not possible to adjust the angle of the extrusion at the edges. But this is easily fixable and preferable to the previous solution.

[lazze]

I have attached a screenshot showing a section of the two shapes I'm working with which are now constructed from a revolve of very clean sketches representing the outside shape into a patch which is then thickened inwards.

(I have no idea why they are drawn in different colors)

[SaeedHamza]

This is a normal thing to happen, since they are 2 different bodies, they will have different hatches with different colors