Descending spiral cut help.

shawnrw

Hello,

Can anyone recommend another strategy for performing the cut below, see first photo? I'm currently using two splines curves to build a surface and splitting/cutting. The second photo is the beginning shape.

Thanks for any help!

steve_shubin

@shawnrw

Did it bit more tweaking of the document

https://cad.onshape.com/documents/d3cc31ef13d8f1f0d070cd04/w/d572fbe44ca72478cb485958/e/e260f7a9b578fec8d322ce38

The red arrows show where to adjust

You can change amounts by quite a bit and it still seems stable

steve_shubin

steve_shubin

@shawnrw

So if you can live with that approx. 5/10,000"s of an inch hump in the middle, than forget everything above

All you need is for the cutter to be horizontal and at 90 degrees to the lathe axis, BUT, raised up above the axis of the lathe as your lathe turns your part

On the last picture below, look at the Y & Z for the Transform Dialog

I don't know why this didn't come to mind before. Getting old and slow of mind. LOL

https://cad.onshape.com/documents/b49b4e9f53fbc3b2b6b578a3/w/c3e1706530117f22abe89193/e/a7b415d68af1cdc7d97c33b5

bruce_williams

Looks like you have it working.  What is the problem?

Please explain and share public doc url for best help.

steve_shubin

@shawnrw

see text at the bottom of this post 

https://cad.onshape.com/documents/d3cc31ef13d8f1f0d070cd04/w/d572fbe44ca72478cb485958/e/e260f7a9b578fec8d322ce38

Here is an alternative method

Read this and see if it’s something you’d be happy with

The variable #r is the radius of the hole. If you need to adjust this radius or the circumference of the hole, do it by editing this variable

The variable #c is the circumference of the hole. This variable is for display purposes. You should not edit this formula

You could adjust anything within Sketch 1 other than the radius of the hole which is the distance from the dashed line to the closed shape. To adjust this distance of the dashed line to the closed shape, do it by adjusting the variable #r

You could adjust anything within Sketch Ramp other than the longest dimension displayed. Because that dimension is set using the variable #r

The GIF shows a section that runs through the dashed vertical center line displayed. In doing this, it doesn’t matter what angle you section from through that centerline. The four points of the two ramps are always going to be at the same height (z)

steve_shubin

@shawnrw

Did it bit more tweaking of the document

https://cad.onshape.com/documents/d3cc31ef13d8f1f0d070cd04/w/d572fbe44ca72478cb485958/e/e260f7a9b578fec8d322ce38

The red arrows show where to adjust

You can change amounts by quite a bit and it still seems stable

steve_shubin

shawnrw

Steve,

Sorry, just getting to this. Absolutely amazing work. This is very helpful! I really appreciate you going above and beyond on this!

shawnrw

Steve,

Ran into another issue, that if willing, I would really like your expertise trying to fix.

Here is a sample part - https://cad.onshape.com/documents/70b760da39aa6a2f37df48f6/w/5c4154d471622de6126dbe94/e/1d4aa30c3adb9c7cf3f99330?renderMode=0&uiState=61b914ed081840488ac27f81

I'm trying to build this helix surface properly so that a verticle .50inch end mill on lather can cut this in one pass while the part is rotated. See the phone for some additional clarification.

steve_shubin

@shawnrw

https://cad.onshape.com/documents/78dc764364262b55b548ab86/w/c6e7cb5e911accb0ef60f81e/e/9b565512fd3075ff6255006b

If your milling tool is oriented radial to the centerpoint of the pipe such as a spoke is to a wheel or a clock hand is to the center point of a clock face, and if that milling tool is also parallel to the bottom of the part such as I have in the various part studios of the attached document, then you won’t have any problem with the cutting tool digging in on one edge, meaning the inner or outer edge of the pipe, provided you use one of the part studios in the attached document as the basis for your model or part

If you look at the attached GIF, I used a plane to cut the face of the ramp in 2 different places. Those cuts are indicated as yellow lines on the face of the ramp. Those lines are parallel to the top plane.

In the GIF below, the yellow lines, and the yellow plane are parallel with one another

The yellow lines are also radial to the centerpoint of the pipe

One of the key things that makes this possible is the Radiate Surface feature script that I used in all of the parts studios. In the case of the attached document, we have a surface that is radiating out parallel to the top plane. On top of the fact that I am radiating out from 180° arc when viewed in plan view or said another way, when viewed from the top.

In the first three part studios of the attached document, I vary the transitions at the top and bottom of the ramp

Part Studio 1 is just a straight line incline. There’s no curve to it at all other than it’s bending around the pipe. But, prior to wrap, the slope is just a straight line with a hard transition at the top and a hard transition at the bottom

On Part Studio 2, I gave a little radius at the top and bottom of the slope

On Part Studio 3, I use a spline that has a soft ease in and a soft ease out at the top and bottom of the ramp, along with there being and overall S shape to the spline as it transitions from clockwise to counterclockwise or vice a versa depending upon how you look at it

steve_shubin

All right. I’m a little slow right now

I think I realize now what you are up against

Give me a little time to experiment and I’ll get back with you

shawnrw

Steve,

If this is your slow, I can't imagine what your fast looks like ! 

Again, thanks for the help, this one has me stumped pretty good... 

steve_shubin

@shawnrw

OK so this is what I got with a half inch diameter round cutter

That’s about as best I can do with all kinds of transformations, rotations, translations. As such, that cutter is not coming off the center of that pipe (not radial) and it’s not even running parallel to the top plane

I’m no machinist

I don’t know how it is that that half inch round cutter would end up taking a little bit off the outer and the inner edge and not touching the middle. That’s completely beyond me. But that’s what I got when doing a Boolean subtract

Yet if I do a section through a vertical line going through the center of that pipe, well where the section happens at the slope of one of those ramps, its horizontal, and that line is straight from inner to outer edge. So how do I get the cutter touching the outer and inner edge and missing the center?

If I were you, I believe there are a number of places online where you can send them your file and they’ll manufacture your part for you because best I could see this is probably going to take a five axis machine. This is beyond me

WAAAAAAAAY BEYOND ME

Some machinist folks should really jump in here on this conversation and let us all know what the heck is going on here

shawnrw

Steve,

You got it a lot close than I have thus far... Just to help build the picture on how we would like to machine it, see the attached photo. Basically, we would have the lathe slowly rotate the part as the spindle moved along the 3D spline line cutting the stock.

I agree, not sure how you are touching the out/inner edges, but not the center portion.... I'm going to try and see if I can't produce the helix in SW with better results; I'll post an update-success or failure.. 

dirk_van_der_vaart

Something like this?
https://cad.onshape.com/documents/7e81d3e326f5092a46f34941/w/174aa5c68f85b60d6e3476a2/e/efba4e6faea3c434442b6358
Not on a lathe, this is with a milling machine.

shawnrw

dirk_van_der_vaart said:

Something like this?
https://cad.onshape.com/documents/7e81d3e326f5092a46f34941/w/174aa5c68f85b60d6e3476a2/e/efba4e6faea3c434442b6358
Not on a lathe, this is with a milling machine.

That is our second option, but the complex helix would better fit the engineering requirements for the design.

steve_shubin

@shawnrw

I think I’ve got an understanding of how this works

Give me a little bit a time to put together some stuff to show you

steve_shubin

@shawnrw

see text at bottom of this post

https://cad.onshape.com/documents/67b7b9d708766ab14c841b64/w/4ae0aed0bde07951d94d419c/e/e12548e591ebb671ef15c95f

So whatever figures, measurements or amounts that are shown in these pictures and in the accompanying document, well those amounts are specific to the slope of the ramp

For instance, if there was no slope, you wouldn’t have to deal with any of this baloney. And I would obviously assume that the closer you get to the horizontal of your slope, that all the measurements and amounts and numbers get closer to zero or 90 degrees. So assume each setup of your equipment to be unique if you have ever changing slopes to your ramps

Along with this goes altering cutter orientation such as the distance the bottom center point is to ride above the outside edge of slope and angle of cutter relative to lathe axis. Realizing that that cutter is not going to be at 90° to the axis of rotation of the lathe, when viewed in plan or overhead

Your lathe would only be at 90° if you were dealing with that which has no slope

But, at least this is a starting point

Now, no matter how you go about it, it looks like there is going to be a slight hump in the middle of the slope going down the center between the inner and outer circumferences. I just don’t know how you can get away with having other than that especially if you want to make one pass with your cutter, and your particular machinery set up. The best I could tell at this point is it looks like that hump in the middle is going to be roughly about 5/10,000’s of an inch higher than the outer and inner edge of the slope. I’m curious to know if this will be acceptable to you

I’m gonna play around with this a little bit more when I have time to give the exact height the cutter needs to be raised off of the outer perimeter of the sloped ramp.

But in the meantime you’ve got this text and the accompanying pictures and the accompanying document to look at

There’s one other thing to consider and it is no small thing. In the example I’ve attached, if you look at the Sketch Slope, you’ll see that the incline is a straight line. That means that once you set the angle of your cutter in relationship to the axis of rotation of your lathe, that you won’t have to alter that angle of your cutter.

But if you were to use a spline that has a constantly changing amount of slope where there is an ease in at the top of the slope and ease out at the bottom of the slope, and then an S shaped curve in the middle, well then the angle of that cutter would constantly have to be changing as best I can figure. And that to me would be a nightmare to try and figure out how to do that.

Now I’ve got to caution you again. I’ve never played with a lathe that I can remember — maybe back in high school wood shop which is a heck of a long time ago. And that type of lathe is obviously a completely different animal from your set up. My background is carpentry, construction and as a builder. Long retired. My interest in geometry comes from cutting in custom roofs and working with structures that are not 90° a lot of times. Out of necessity, I had to figure how to get everything to fit together. So be sure to take everything I’ve babbled on about here with a truckload of salt. Not a grain — but a truckload

steve_shubin

@shawnrw

So if you can live with that approx. 5/10,000"s of an inch hump in the middle, than forget everything above

All you need is for the cutter to be horizontal and at 90 degrees to the lathe axis, BUT, raised up above the axis of the lathe as your lathe turns your part

On the last picture below, look at the Y & Z for the Transform Dialog

I don't know why this didn't come to mind before. Getting old and slow of mind. LOL

https://cad.onshape.com/documents/b49b4e9f53fbc3b2b6b578a3/w/c3e1706530117f22abe89193/e/a7b415d68af1cdc7d97c33b5

shawnrw

@steve_shubin

I think your work is incredible on this in Onshape, but sadly I think we are limited to what Onshape is capable of until a swept cut with body type feature is integrated/created. Check the link out below and let me know your thoughts... I cheated a little and used SW to produce the correct helix surface and used an imported body to subtract the shape in Onshape.


https://cad.onshape.com/documents/db752e827fde32c6bcbfca0c/w/de08d34c4046cd26b25dbb25/e/88104f14e3abf54a93d41797?renderMode=0&uiState=61ba84ac7620976f43dd4bd0

steve_shubin

@shawnrw

That’s a neat tool that SolidWorks has

I would like to see that in Onshape. I think that would be a nice tool to have in the collection 

But you should be aware of that SolidWorks tool’s limitations.

Using your SolidWorks part — I made a section that was radial, that came off the center of the pipe approximately in line with where you showed your drill bit

Now my latest method using Onshape yielded an upward bow between inner and outer circumferences along the radial of approx. 5/10,000 of an inch

On the other hand, the SolidWorks part has an upward bow of 8/1000 in the middle.

So SolidWorks bow appears to be over 10 times worse than what Onshape can do, that is if you’re going to use that CAD tool that SolidWorks has

My method has the same Z height where the radial intersects the inner circumference and the outer circumference

Again, SolidWorks inner is .043 inches lower then at the outer circumference. So their path is not level along the radial with regards to the endpoints

Onshape’s endpoints are level

SolidWorks are not

Onshape has a relatively minor bow

SolidWorks has over 10 times the bow

Myself, as it stands right now, I would not be too quick to import anything from Solidworks regarding what it is you want to do. From what I’m seeing, it looks a lot less accurate than this last method I showed using Onshape

But maybe what that SolidWorks tool is doing is exactly what you’re looking for.

And there’s always the fact that I may be missing something. After all I have been kind of slow of mind lately.

Anyway — let me know how it turns out

steve_shubin

Graphics regarding the above post

The below is a result of using a particular SolidWorks tool
It might be just what you are looking for.

On the other hand, if you are looking for zero degree side slope and little or no camber ...

steve_shubin

@shawnrw said:

I think we are limited to what Onshape is capable of until a swept cut with body type feature is integrated/created

Thanks to @konstantin_shiriazdanov Onshape can also get the same results as SolidWorks swept cut with body type feature

There are 3 of Konstantin's FS tools in this document ---
Sketch wrapper
Normal surface rib
Cylinder sweep

I found that ver.4 of Normal surface rib is what I had to use
I couldn't get version 5 of Normal surface rib to work

https://cad.onshape.com/documents/0fd38c86e4e8fdd639c01bc5/w/82ad0240edcb41fe2034db16/e/f6e13b2bd4d4aeea640e1376

konstantin_shiriazdanov

@steve_shubin I've made some breaking change in last version of surface rib, so that it broken the support of nontangent edges. But happily now we have Ruled surface that I would personally recommend

steve_shubin

@konstantin_shiriazdanov

I appreciate your pointing me to the ruled surface FS. For some reason I was not aware of it. It looks like it has some nice features such as angle

But for what I did in this latest document, your Normal surface rib v.4 is much better.

Your Normal surface rib has a second direction (Side 2 length). This allows me to use less steps

I tried using ruled surface, but the surface it created did not extend inward enough. As a result, when I used cylinder sweep, part of the inside face of the pipe still projected upwards

Thank you for the tools you have made and the help you’ve given here in the forum

shawnrw

Hello,

Does anybody know if the new "SWEEP PROFILE ORIENTATION" feature would help accomplish this cut? I'm trying to create a proper mill/turn cut as discussed above. Currently, I have to take the part to Solidworks to perform correctly.

https://forum.onshape.com/discussion/22423/improvements-to-onshape-december-15th-2023/p1

Thanks,
Shawn