Challenging geometry problem

[SPerman]

I have a challenging geometry problem, if anyone is interested.

We have a sensor bracket that we attach to the column using magnets. Under certain conditions, if bumped in the right way, the bracket could come off. The solution we hit upon was to rotate the bracket as it is installed on the machine. This is working well. The "arms" keep the bracket close enough to the column that even when hit, the magnets keep the part in place.
I am a GIF! Click me.

It turns out, for me at least, modelling the cutter part to create the appropriate geometry is a significant challenge. My solution was to create an array of columns and join them into a single body to use as a cutter part. This means I know have 3 parts and 1 assembly to create this bracket. It also means there is lots of tessellation on the faces, which adds to the challenge of filleting.

image.png (25.95 KiB) Viewed 703 times

I spent over a day trying to both understand and model this geometry. I eventually gave up and went this route. We are moving forward with production using these models, but I'm hoping one of the surfacing guru's has a better way to accomplish this.

I will add the solidworks files as soon as the forum allows it.

[SPerman]

Here are the files.

BRACKET.zip

(5.14 MiB) Downloaded 7 times

[TTevolve]

Start with a circle the size of the OD or ID.
Make a helix - you can use pitch and revolution or height and rev if you want (in picture below 0.25 of 4 " pitch is 1" overall height - do height/rev if you want the height fixed)


Sketch a line and do a surface sweep along the helix

Sketch the pie shape and extrude up to surface

You can add the ID hole as a straight cut or add it to your extrude sketch if you wish

[SPerman]

A helix does not properly describe the geometry.

(I couldn't figure out how to make a helix work, anyway.)

[bnemec]

A helix does not properly describe the geometry.

(I couldn't figure out how to make a helix work, anyway.)

Helix was my first thought. Attached my first thought. Your files are in a newer version than we have or I would overlay them to see the difference.

[AlexB]

Have you looked into a solid swept cut? I am trying to attach files and screenshots but it seems to be broken...

Edit:

2024-05-13 14_02_00-SOLIDWORKS Premium 2023 SP5.0 - [Tubing Rotate Cut.SLDPRT].png (138.92 KiB) Viewed 623 times

[SPerman]

I've probably overlooked something obvious, and you guys are going to make me feel silly.

A helix still seems like the logical solution, but I couldn't make it work.

I did try a sweep with a twist, but that didn't seem to work. I also tried a straight extrude and applied the flex, but it did weird things to the faces.

The forum is definitely having issues with attachments today. (https://www.cadforum.net/viewtopic.php?t=3429)

[AlexB]

I've probably overlooked something obvious, and you guys are going to make me feel silly.

A helix still seems like the logical solution, but I couldn't make it work.

I did try a sweep with a twist, but that didn't seem to work. I also tried a straight extrude and applied the flex, but it did weird things to the faces.

The forum is definitely having issues with attachments today. (https://www.cadforum.net/viewtopic.php?t=3429)

Updated my post above with attachments

[bnemec]

Any hints on how they machined that part in your gif? The cut face shape is not matching what a swept solid tool cut on helix profile (like AlexB has). I tried sweeping the post out on a radial helix like Alex shows but doesn't match physical part. I also tried sweeping an "end mill" aligned radially to the tube with a helix axis on the tube axis but that still doesn't match what you have.

[SPerman]

Have you looked into a solid swept cut? I am trying to attach files and screenshots but it seems to be broken...

That looks like it will work. When I have time this evening I will dig into it deeper.

[SPerman]

After looking at it further, the geometry created is close, but not identical. I will have to print one and see if the differences still allow it to rotate on the way it is supposed to.

I was unaware of the ability to use a body during a swept cut. (Am I correct that this functionality is only available for a swept cut, and not a sweep?) I was hoping to make a solid body using the swept solid to help me visualize the shape, but it doesn't look like I can do that.

[SPerman]

Any hints on how they machined that part in your gif?

Additive manufacturing (i.e. 3d printed.)

I tried sweeping the post out on a radial helix like Alex shows but doesn't match physical part. I also tried sweeping an "end mill" aligned radially to the tube with a helix axis on the tube axis but that still doesn't match what you have.

My part was created by creating an array of columns, with a linear translation/rotation between each one, and using this as a cutter. In my mind, that geometry has to be correct. It absolutely represents the relationship between the bracket and the column at each position, and it has been confirmed to work in the real world, as shown in the GIF above. The fact that the swept cut doesn't match this array of tubes makes me think the swept cut is wrong, but since I've just learned about this tool maybe it can get there.

image.png (82.46 KiB) Viewed 569 times

[AlexB]

After looking at it further, the geometry created is close, but not identical. I will have to print one and see if the differences still allow it to rotate on the way it is supposed to.

image.png

I was unaware of the ability to use a body during a swept cut. (Am I correct that this functionality is only available for a swept cut, and not a sweep?) I was hoping to make a solid body using the swept solid to help me visualize the shape, but it doesn't look like I can do that.

Currently it's only used for a swept cut, but you can get the solid version if you create a large bounding body and make a copy of it as well. Then apply your swept cut to one of the bounding bodies. Finally Combine -> subtract your cut bounding body from the original bounding body.

New body after subtract combine

image.png (75.53 KiB) Viewed 563 times

[matt]

Yeah, the swept solid cut sounds right. You may have to use a straight line for the path and the helix centerred on the line as a guide curve to get it to twist correctly.

[SPerman]

I took the time to make sure I am comparing apples to apples, and tweaked the helix parameters, and the geometry is the same.

Thanks again for everyone's assistance with this.

[TTevolve]

I did see something the other day about a wrap cut - here is the link to video for it.

[SPerman]

There is a minimum pitch for the helix, below which the swept cut will fail.

[SPerman]

If you get close to that limit, it creates strange discontinuities on the cut face.

[TTevolve]

You can do curves in other ways then the helix, it's just the fastest and easiest if you have a regular ramp shape to do it with a helix.

you can use planes and sketch with reference geometry to make your curve

You just have to have a surface to either extrude or cut to to make the ramp solid you want.