How to Bend an Extruded Part

Warren

Apologies for this simple question but I've searched docs and forum and cannot figure this simple geometry..

I have a flat washer (2 circles of differing sizes, sharing a center point, and extruded to give thickness).
I would like to "bend" this flat washer against a large arc (a portion of the circumference of a large circle, sketched perpendicular to the washer).. much like if you were to bend a small flat washer onto the surface of a larger pipe.

The key is that this geometry must "bend" correctly such that the edges of the washer stay perpendicular to the face of the washer.. I am stumped.


 

brucebartlett

Create a part with a curved top surface using the side profile and top profile. Then use the thicken command by selecting the top surface of first part, edges will come out normal to the curve, Make sure you select New at the top and you will end up with 2 parts.

philip_thomas

Just for poops and giggles I wondered what a generic solution might look like. Here is a public document that you might pick up some ideas from
https://cad.onshape.com/documents/f6766b6cad2f496f89e0115e/w/8633fd371c854192aacaf150/e/77a25806418942a29625b12a
I hope this helps

brucebartlett

Create a part with a curved top surface using the side profile and top profile. Then use the thicken command by selecting the top surface of first part, edges will come out normal to the curve, Make sure you select New at the top and you will end up with 2 parts.

Warren

Thank you Bruce. I certainly would never have approached it that way. Much appreciated.

philip_thomas

Just for poops and giggles I wondered what a generic solution might look like. Here is a public document that you might pick up some ideas from
https://cad.onshape.com/documents/f6766b6cad2f496f89e0115e/w/8633fd371c854192aacaf150/e/77a25806418942a29625b12a
I hope this helps

Warren

Thanks Philip. That actually solves a similar problem I could not figure out. Extrude through a thickened surface, and take the union. Thank you very much for this; very helpful.

onshaper

I like these solutions, but they are inaccurate. Original washer is 6820 mm^3, bent washer is 7440 mm^3. That's a 9% increase in volume.

Warren

@Onshaper that is true. Also, the thickened extrusion union will not have edges of washer normal to surface (they will not be square with the face of the washer).. but it is close depending on the application. The solution from @BruceBartlett is closest, the only issue is in creating the initial geometry for the actual parts becomes quite onerous. I used the example of a washer as the most simple way to describe the problem, however in practice the actual part to be bent is more complex. In a perfect world, being able to snap a surface to an arc would be the most straightforward; much like lofting, except with the loft path acting parallel to a surface rather than perpendicular.

andrew_troup

The other 'cheat' in @Philip Thomas 's intriguing (but unrealistic) solution is that he uses a spherical rather than cylindrical form, so that the washer is not bent but 'drawn' (multiaxial or compound bending). This craftily gets around the problem of mapping a circle onto a cylinder, because when you map it onto a sphere, it remains a plain, planar circle.

To achieve the OP's task, in (say) Solidworks, I guess one would create a cylindrically curved surface representing the neutral axis of the finished washer, use "wrap" to transform a pair of concentric circles onto the surface (in a way which preserves the circumferential length and curvature), trim away the excess, then thicken the resulting surface in both directions, biased by the k factor appropriate for the process?

I can't see a viable way of doing that in Onshape right now, in the absence of 3D sketches. Anyone see how this could be done in a not unduly laborious way?

philip_thomas

@Andrew_Troup - yes, my solution will be larger than true life because I am projecting and not wrapping. These sorts of capabilities will come, but we have a lot of stuff to work on so please be a little patient with these corner cases.

onshaper

I have a lot of faith in Onshape. I hope we can have true bent parts and... CAM and sheet metal and frame and structural FEA and dynamic analysis AND AND AND  

andrew_troup

@Philip Thomas - I'm more than willing to be patient. It's one of my faults.   My question was designed to elicit ingenious workarounds in the meantime from other users, not to put pressure on for more functionality; seems to me it's arriving faster than anyone has any right to expect, and at a good rate to permit user familiarisation in real time.

Warren

Yes, @Philip Thomas  I certainly understand and agree with the development priorities; I'm very satisfied with the features in Onshape thus far, taking into consideration the relative newness of the product. Just doing my "part" (ha ha) to attempt specific characteristics of my models where I know they can be a challenge. I also have expectations for Onshape more along the lines of SolidWorks, vs. something like TinkerCad.

philip_thomas

Sorry - I hope that no one felt that I was being defensive. We have some very bright people and the input from thousands of users and we wish we could do everything right now. On the plus side, we are very agile and the functionality that you are seeing is just the tip of the iceberg. There is stuff running on our internal servers that is really amazing and i cannot wait to show it to all of you. #goodstuffcoming

3dcad

@Philip Thomas  I really like and appreciate your quality aspect not to release new features before you think they are ready. The few bugs I have bumped in Onshape has been very minor and the software has developed in amazing speed.

We try to give you all the ideas we have in earliest point when you can think of them while building up the frames so that there is support for everything when the time is ready for corner cases.

Keep up the good work.

aaron_clark

Not having the bend/flex tool is the only thing holding me back from converting my business from SW 2011 to Onshape. Can someone let me know when that tool is available?

rune_thorsen229

I vote for a solution here because I need it too. Several times I have come across the need for designing a flat object (cloth, rubber etc) that would be folded around another object.
Any news?

chandran_palanisamy

Not sure this helps directly but worth considering as a workaround. I wanted to create a curved arrow with a curved arrowhead. The arrowhead was challenging and I did the following steps to get it. it looks good and you can see all the details at the link below as it is a public drawing.
1. A construction circle of dia 25mm in the 'Front' plane.
2. A rectangle of 10x1mm in the 'Right' plane.
3. Revolve the rectangle in the Right plane for 270 degrees.
4. A construction circle at the origin of 12mm dia. A circumscribed polygon with 3 faces.
5. Extrude the triangle by 1mm.
6. Replace the Triangle face with the (revolved) curve's outer face from the 3 above. Now the Triangle's one face will be curved and the other will be flat and the Triangle's thickness gets increased.
7.  Delete all other faces except the curved face of the Triangle, which now appears as a continuation of the curve.
8. Thickene the curved face by 1mm.
9. Boolean operation Union to merge it.

If it feels like a Rue Goldberg's style process, my apologies as I am still learning OnShape. I would love to hear easy ways of doing the same.

https://cad.onshape.com/documents/4ce85ceff93f127cc503c89a/w/9c36946fb077d51f38385a92/e/c2b4b0a201956e67c032602d

chandran_palanisamy

Not sure this helps directly but worth considering as a workaround. I wanted to create a curved arrow with a curved arrowhead. The arrowhead was challenging and I did the following steps to get it. it looks good and you can see all the details at the link below as it is a public drawing.
1. A construction circle of dia 25mm in the 'Front' plane.
2. A rectangle of 10x1mm in the 'Right' plane.
3. Revolve the rectangle in the Right plane for 270 degrees.
4. A construction circle at the origin of 12mm dia. A circumscribed polygon with 3 faces.
5. Extrude the triangle by 1mm.
6. Replace the Triangle face with the (revolved) curve's outer face from the 3 above. Now the Triangle's one face will be curved and the other will be flat and the Triangle's thickness gets increased.
7.  Delete all other faces except the curved face of the Triangle, which now appears as a continuation of the curve.
8. Thickene the curved face by 1mm.
9. Boolean operation Union to merge it.

If it feels like a Rue Goldberg's style process, my apologies as I am still learning OnShape. I would love to hear easy ways of doing the same.

https://cad.onshape.com/documents/4ce85ceff93f127cc503c89a/w/9c36946fb077d51f38385a92/e/c2b4b0a201956e67c032602d

james_brown918

I'm fairly new to OnShape and to CAD but wouldn't the simplest method be to use Plane to create a new plane, draw the circles for your washer on the new plane and then use the Wrap to place it on the cylinder and define the thickness? 

Sketch 1 is the cylinder. Plane 1 is defined as an offset from Front that is beyond the circumference of Sketch 1. Sketch 2 is the outer and inner circle for the washer. The Wrap places it on the curved cylinder and defines the thickness. Part 2 is the washer.

https://cad.onshape.com/documents/6ab7e0d28af6562a2ca29210/w/13b53a03e4ddaa4423d8bba2/e/c65c27803be6e4d785456a40?renderMode=0&uiState=620cd343fe7b4734eaece347

james_brown918

Chandran---
For an arrow similar to yours, I did the following:
Sketch 1 is a cylinder on the Top plane with a diameter of 25mm extruded to 25mm. This creates Part 1
Plane 1 is a new Plane offset from the Front plane by 30mm.
Sketch 2 is an arrow on Plane 1. I didn't measure. I just drew it.
Wrap 1 wraps the arrow around the cylinder and defines the thickness as 1mm. This creates Part 2.
Then I hid Part 1 leaving Part 2. Or you could Delete Part 1.

https://cad.onshape.com/documents/7bc0c7e98f70b72416b7da06/w/f48c8a71cc27c3573fe96509/e/d647fe4e9a70ccf900db525a?renderMode=0&uiState=62078c5df63c323f0b4be3b9

NeilCooke

There is also a custom feature that creates arrows for you
https://cad.onshape.com/documents/b1d910f6c2407f9e1ec854e5/w/9c24518f2e1fc47944dac6d6/e/b9767832ada4bbffa318c31b