Looking for modeling technique suggestion: Sweeping a variable profile using 2 different sweep paths

StephenG

I am trying to model a replacement cover to a set of microwave cookware. (Replacement cover is no longer available. I plan to print a replacement on my new 3D printer.)

Is it possible to sweep a profile whose ends are connected to different paths?

Note: One curve in the profile is partially constrained to allow the profile to reshape itself as it is swept along the 2 profiles.

I have done this type of surfacing in other CAD systems, just want to know if Onshape (in its present state) can do it. I cannot figure out how to effect it.

If it cannot be done I am guessing I will have to revert to manually constructing a series profiles and lofting the surface.     

NeilCooke

@stephen_gertsch sweep only works with one profile. I would remove the R1.25 and make two sweeps, then add the rad back after. You could also build the final shape using 3 extrudes and 2 fillets.

StephenG

I forgot to include a picture...

NeilCooke

@stephen_gertsch sweep only works with one profile. I would remove the R1.25 and make two sweeps, then add the rad back after. You could also build the final shape using 3 extrudes and 2 fillets.

StephenG

Thanks for the technical tip: do 3 separate sweeps. I attempted to loft the surface abut ran into other problems.

I really like your suggestion.

Note: I created a "Branch" for the 1st time. I created a branch to isolate using a different modeling approach to create the surface. Up until now I have simply "Duplicated" the Part-Studio to try an different modeling approach. I am beginning to appreciate the power of branching.

StephenG

Well..., my first attempt didn't work so well; there are gaps along one surface.
(Actually, I did 2 sweeps: 1 sweep for the outer and 1 sweep for the inner surfaces, then a loft to connect the 2 surfaces.)



Tried using the edge of the existing surfaces as "Guide Lines" but the "loft" would fail. Going to read up on use of guide lines.

NeilCooke

Does it have to be surfaces? Currently there is no join feature which will make this tricky. If you can share a version of the doc I can show you how I would do it. 

Tony_C_

stephen_gertsch said:

I forgot to include a picture...

I'd try that using loft.  

Get rid of the bottom half of your paths so you just have the top 180deg then place a copy of your sketch at 9,12,&3 O'clock. Choose those as your loft surfaces and your inner/outer sweep paths as the rails. 

StephenG

Nailed it! Amazing what you can learn by reading the documentation.

First problem: I selected edges of the surfaces as guides. Guide curves have to be their own sketches (Why?)
Second problem: I created the projected edge lines as construction line type; they need to be "solid". (Why?)

Now you tell me I cannot join/merge the surface patches into a single surface. Oh joy.

I will share the Document with you so you can show me how you would do it...

From what I can determine you (OnshapeSupport) should already have access to it.



I tried explicitly sharing the Doc with you "NeilCooke" but it wasn't recognized.

NeilCooke

If I knew the design intent I may have modeled it different, but here is one way to do it: https://cad.onshape.com/documents/58ab5bd4b689510fc5a83aa4/w/f2482a2fe5d353ebb7ead234/e/1480953e4ffa870b10846ef5

owen_sparks

Just a word of caution, if you intend using this part rather than using it as a CAD exercise.  What material are you intending to print with?  PLA may well go floppy, ABS tends not to be food safe etc.  (I've seen chocolate moulds 3D printed so some is safe.)

Regards,

Owen S.

michał_1

@stephen_gertsch you should follow @NeilCooke first idea 3 extrusions and 2 fillets (maybe one more extrusion to get lip). There are no reasons to use surface modeling, going your way it's like asking for troubles. All features on that cover can be done with solid modeling and they should be.
It is very important to know when to use surface modeling. Even if you have "organic" shape all features that look "prismatic" should be done with solid modeling, after you finished with surfacing.

Ben_

owen_sparks said:

Just a word of caution, if you intend using this part rather than using it as a CAD exercise.  What material are you intending to print with?  PLA may well go floppy, ABS tends not to be food safe etc.  (I've seen chocolate moulds 3D printed so some is safe.)

Regards,

Owen S.

Owen, some of the PETG filaments are quite robust in this context. Some are food safe higher melting point and tougher than other types of filament. Still a good point to make as ABS and PLA are not really suited to food applications

owen_sparks

@Ben_

Thanks Ben, I appreciate the i@Ben_
Cheers, Owen S.

StephenG

I am doing fit interface checking with PLA and intend to try clear PETG for the end product.

My real problem is that my 3D printer is too small to print the full size part. I isolated the critical interface feature(s) and "pie" cut the model in 3rds and glued them together to complete the fit check. I am glad I did because I had to tweak a couple of dimensions to get it to fit exactly as the original with its "wiggle room" clearance. I used a "branch" to isolate the main model work from what had to be done to it (pie cutting) so I cut complete the fit check. Branching worked well for this purpose.



I checked around at local 3D printing services and I got a quote of $290 to print the full up model.  I am committed to getting this thing made, but I am not $290 committed. I will resigned the model to be an assembly of parts that I will glue together. I will add additional features (channels matting edges) to facilitate the assembly.

I just finished up the base model by adding the vent/drain feature.


The vent/drain feature was little trickier to build than I thought it would be. I spent some time finding the right number and application order of fillet operations to get the thing done. 

All in all, this has been a fun exercise in learning to use Onshape and my new 3D printer.

mahir

3D printing costs are due to size, material volume/weight, and printing time. Basically, you have to pay for the plastic and also rent the room in the printer while it's printing. Your overall size is what it is, but if the design can take it, you can reduce the 3D print cost by making the whole thing thinner.