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Merging two profiles into one whilst sweeping two different lines
aaron_simmons
Member Posts: 5 ✭
Hi,
I am stumped on how to do this but I need to merge two different profiles whilst they sweep along a separate upper and lower line.
Its basically an oval shape going into a round shape but the oval need to increase in size as it merges.
I am trying to draw this up from a 1960's hand drawn engineering drawing of something that I would like to recreate.
Pictures attached, the blue arrows are the sweep paths needed.
Best regards
Aaron
0
Comments
Your going to run into self intersecting errors because of that top sweep arc. imagine what will happen to the circle as it tries to stay perpendicular to that arc. the bottom of the circle will travel backwards past other geometry. Have you tried loft with guides?
I have but no luck!
Here is a link if anyone would like to give it a go
https://cad.onshape.com/documents/e7bcca8eb274edb3cebd070d/w/71dce084c866aadcd0bf75e5/e/d287c0caebfadd92611815b8?renderMode=0&uiState=679e4bdb026426762180a156
Here's a screenshot to study and attempt. it. Highly reccommend spending some time on learn.onshape.com for more help on loft functionality and more. pretty advanced feature if your new to such things.
Loft with guides will work, but you'll need to fix Sketch 5 if you want to use those intermediate profiles (Sketch 5 is not exactly coincident with the top/bottom guides created in Sketch 2). The resulting shape is very constrained (profiles AND guides) and does not flow very naturally…
If you just want to use the start and end profiles then it works fine, but the shape is also a bit odd as it is still being tightly constrained by those guides. The guides are also only tangent connected (line segment into an arc) which means the curvature transitions are a bit abrupt. This may or may not be an issue depending on the end goal.
I created the outside loft here https://cad.onshape.com/documents/31790452d77354b034ba2472/w/7fadec76354784e9bbc16e8b/e/1eb5cd48549d74ff30d4ea0e you can probably just thicken 0.05" it to finish the solid shape
If I were you, I would start with only the profile and guide curve sketches (delete the extrudes). Then loft as a surface, the two outermost end profiles using guides curves (one continuous loft) - thicken that surface to the correct thickness, then add those little webs last. I would also recommend that you edit the guide curve sketch, and reduce the number of picks where possible (replace two straight lines with one) this just makes the selection process a little easier.
The trickiest part is the multiple edge selection for the guide curves. Each selection set (multi part guide curve) has to have there own bounding box in the UI. If you don't understand this, take a refresher course in the learning center, paying attention to selection process.
MDesign has basically shown how to do this. And he is right about this being advanced skill level, but this is how we learn, is it not? Stay with it.
Thank you all!!! I now know where I was going wrong!!!
I've not really played with doing lofts but i will look up doing some more learning.
Once again thank you all!