Wrapping a swept profile around a cylinder in Alibre Atom

I am progressing albeit slowly with my design for a 5 - speed sequential gearbox and have got to the stage of trying to produce models for the gear selector drums, Now, here's my problem. I have sketched out the desired features for the selector forks to follow in 2D, by drawing a profile and using the sweep function. I cannot find a way to wrap the path around a cylinder so that the profile follows the desired pattern. Any ideas?

I've Googled and looked at the Atom forum but as soon as you type in "wrap" all it seems to come up with is to do with text.

I should add the I'm producing the resultant parts on my 3D printer which I'm slowly getting to grips with.

Here's what the design looks like so far :

John

John,

I'm not really clear what you want to achieve. Do you have pictures of a similar part??

The Wrap tool in Atom3D will work with any sketch (text or otherwise) - but be careful of getting too close to the edge of the target.

Depending upon exactly what you need to achieve, 3D sketches might be needed (not supported in Atom3D).

You might get further by posting a query on the Alibre user forum (do mention that you are restricted to Atom3D) or even by submitting a support request to Alibre.

Based on your title, you can't wrap a swept profile, only a sketch.

Edited By David Jupp on 26/09/2023 11:16:30

Edited By David Jupp on 26/09/2023 11:16:49

Edited By David Jupp on 26/09/2023 11:18:26

If it's a cylinder it has an axis you can revolve the profile sketch around

So use revolve boss, not sweep

and start with a simple square sketch, make sure it revolves, then edit the square into the complicated drawing you require

edit: All looking very nice btw

As David says, you may have to break the part down into a revolve boss and then a pattern cut

Edited By Ady1 on 26/09/2023 11:31:28

And I hope that drawing is an assembly of parts, not a single part

If you want to revolve an extrusion use the circular feature pattern

Edited By Ady1 on 26/09/2023 11:36:51

Anything like

That is just a wrap of a sketch around the cylinder, can be tidied up by adding fillets to smooth out corners.

Edited By David Jupp on 26/09/2023 11:36:19

Edited By David Jupp on 26/09/2023 11:37:16

Atom3D Help has a non-text example (just a simple rectangle), but it gives the basic idea. The sketch to wrap can be more complex.

The Framework of Wrap (alibre.com)

Thank you for your replies and hints.

David, the solution shown in your second response looks to be just the job. I'll try that after lunch as well as having a butcher's at the Framework link.

This is part of a Hewland FTR sequential gearbox selector barrel part 45 :

And this is what I've done on a plane surface by drawing the path and then the profile on the plane at right angles to the path followed by an extrude cut along said path.

Doesn't look too dissimilar to your example, David, so my hopes are high!

Ady 1. Yes, that is an assembly screen grab. I dread to think how long something of that complexity would take to print as one job, even with my high speed Bambu Lab X1 carbon printer! And just imagine the support structure that would be needed.

Regards, John

John,

To save time, and make it easier to edit later, I'd suggest just use straight lines in the sketch. Use 3D fillets afterwards to smooth changes of direction, and to round the sharp corners at bottom of the groove.

Looks like an awkward one that really needs the 3D sketching function

Us poverty stricken Alibre Atom serfs can do a workaround by using multiple planes, but it's a slow process

I've done the first plane and cut, then a plane at 20degees(?) would do my next cut etc

All very fiddly

Can Alibre Atom now do sketch wrap?

I'm stuck on V25

Wrap was introduced with v25, ah but sorry NOT in Atom3D.

Apologies for not spotting that earlier.

David,

Yes. Me too. I can see how to do it in Alibre design but of course the wrap function is not available in Atom. Thanks for trying any way.

Back to the drawing screen for a re-think and maybe a modified design.

John

P.S. Can't figure out if it's possible in Fusion 360 either, if that's any consolation.

A work around in Atom would be to treat each part of the groove as a separate operation applying different cuts to each. The main straight groove could simply be sketched onto a plane and then cut. The ones where the grove runs at an angle would need to be done with a helical cut for each angle so you would need to do that in three operations.

Once you have these done then as David says add the fillets as a separate item.

Here is a rough one done as described above, the three angled parts of the slot are helical cuts, the rest a revolved cut. Fillets added to internal and external corners though the external need looking into some more a sthey are not right. All options that are available in ATOM. I suggest making the groove deeper than needed and then extruding a solid cylinder to bring the bottom out to the correct depth.

Pitch of the helical cuts needs to be pi x outer diameter assuming 45deg angles. When sketching the rectangle for the helical cuts make it 1.404 times the width of the straight groove again assuming 45 degree angles. I simply used 14mm and 10mm in the example and a 100mm dia with 314mm pitch to the helix

Edited By JasonB on 26/09/2023 14:54:19

Jason,

I THINK i understand what you're getting at, except for the straight bits.

I think i might try doing it piecemeal using revolve cuts in angular sections and then joining them with helical cuts as you suggested. Come to think of it, it would probably be easier to do that the other way around. I'll have a go later when my brain has cooled down and report back on my progress - or lack thereof.

John

Jason,

My page has just updated to show your 14.50 reply. That looks promising. I'll have to see what I can achieve in Atom.

John

Off to watch your video..........

Nice solution Jason (my brain only slightly exploded)

Jason beat me to it - whilst out of office I thought of the combination of revolves with helical cuts.

Not sure why you'd need to make grooves deeper, then fill in though - but whatever works for you.

Using 'project to sketch' from flat face of one end of cut can give starting sketch for next section.

David, I may be possible with a bit more work or positioning the sketches differently but I was getting a "step" in the bottom of the groove where the straight one met the helical.

By effectively filling the bottoms those steps become part of the solid

Yes I created a plane at the end of the first angled cut then projected the sketch to be extruded for the next part.

Jason,

If you get steps then I absolutely see the logic of your approach.

It is possible to avoid steps, but may not always be practical to do so (I am aware of one possible flaw with the simple example shown, that would take some careful thought to get around).

The groove shown has slightly different width across the slot for the helical vs straight sections.

Edited By David Jupp on 26/09/2023 16:04:47