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Solid Sweep (Cut): Designing a Feedscrew

Question asked by Iain Hendry on Jan 16, 2013
Latest reply on Dec 19, 2014 by Eric Husted

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Hi all,

I've done some digging around in the forums, but can't seem to find an answer to what I'm trying to do and having some difficulty with.

What I'm trying to do: I'm designing part of a machine which consists of a feedscrew; each revolution of the screw advances one part along a conveyor. The part is basically an extruded oval.

Making a Helix and then sweeping the profile of the part along the helix doesn't work, because the material left over on the screw interferes with the part a few degrees before and after the point of engagement.

I understand the use of Solid Sweep (vs. Profile Sweep), and Solid Sweep should give me the effect I'm looking to create. However, Solid Sweep seems to only work with a cylindrical solid, not any other shape. As my part is an extruded oval, I can't quite think of a workaround for this.

Any suggestions? Attached is a part file showing the dilema - I want to make a Solid Sweep (Cut) using the body "Part Representation" and "Helix/Spiral1" features, but it won't allow me to make the feature.

Thanks in advance!

-Iain

(SolidWorks 2012, SP5.0)

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Feedscrew 1.SLDPRT.zip94.4 KB

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1-4EQZK9 Jan 16, 2013 10:43 AM
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Hi Iain,

the solid profile is not valid for a solid sweep cut. See attached. I'm not sure what version you are on so you might not be able to read it (I did the attached in SW2012) so I provided to screen images. Frankly, Think of Solid Sweep's primary use as a tool for cutting using a rotary tool. - thus, I do not see how you would use the profile you created as a tool for cutting in real life?

Regards

Mark
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- Feedscrew 1-mab.SLDPRT.zip832.3 KB
- solid sweep 1.png352.9 KB
- solid sweep 2.png265.6 KB
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Iain Hendry @ 1-4EQZK9 on Jan 16, 2013 11:30 AM
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Hi Mark,

Thanks for the reply; I wasn't able to open your file, even though I'm using SolidWorks 2012 (SP5.0). But I can tell from your .PNG images that what you have shown would generate the same geometry for the screw as a Profile Sweep Cut, which won't work for what I need to do.

Here's a video showing a similar setup so you can imagine what I'm trying to do: http://www.youtube.com/watch?v=lDafdnAi-Z0 (this is a bit more complex than what we're doing, but it's the same sort of idea). I've attached two files, as if the part that needs to move along the conveyor is a cylinder (not an oval). You can see the difference between Solid Sweep Cut and Profile Sweep Cut. Profile Sweep Cut has interferences between the part and screw, while Solid Sweep Cut does not.

So, I need to make a Solid Sweep Cut of my oval-shaped part along the screw, but am not able to figure out how to do this.

-Iain
Attachments
- Profile Sweep Cut.SLDPRT.zip108.9 KB
- Solid Sweep Cut.SLDPRT.zip704.6 KB
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Niven Le @ Iain Hendry on Jan 18, 2013 2:53 AM
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Hi Hendry,
I may have misunderstood here, but I believe that you want to have the left over material from using sweep in order to achieve your design purpose.
Another way method I would suggest is to widen your sweep profile, then sweep.
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Nicolas ALEXIS Jan 18, 2013 5:01 AM
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Hi Hendry

I'm trying to do the same thing, the problem is that you have 2 straight lines in your sketch, try to replace these lines by circles with large radius.

Be careful with solidworks 2012, Solid Sweep function has a bug 671077 "Solid body sweep cut along helical path produces incorrect result".
Attachments
- vis_forme1.JPG95.0 KB
- vis_forme2.JPG129.6 KB
- vis_forme3.JPG102.9 KB
- vis_forme4.JPG107.4 KB
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Iain Hendry @ Niven Le on Jan 21, 2013 8:02 AM
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Hi Niven,

Certainly, that is an idea - however, it would not produce a "perfect" geometry - it would be a comprimise.

-Iain
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Iain Hendry @ Nicolas ALEXIS on Jan 21, 2013 8:07 AM
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Hi Nicolas,

I tried your suggestion, but without success. The feature still fails for me in the selection stage. It certainly does look like we are trying to accomplish the same task!

I've attached the file with the file I tried with - I tried many different radii but it would not solve. I tried only extending the Boss-Extrude2 feature in one direction, or changing all sorts of dimensions (wondering if it was simply "on the edge" of working) - to no avail. I want to use Helix/Spiral1 as the path, and Boss-Extrude2 as the material with which to cut.

-Iain

SolidWorks 2012, SP5.0
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- Error.jpg293.6 KB
- Approximation.SLDPRT.zip93.6 KB
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Matt Neuman @ Iain Hendry on Jan 21, 2013 9:02 AM
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Hi Iain,

I think you need to look at the suggestion Mark Biasotti made above, that is the only way to get Solidsweep cut to work predictably. I'm not sure how Nicolas got it to work with that shape, I have used Solidsweep cut extensively and only been able to use cylinders. i have attached a sample like Mark showed, but in SW2010 so you should be able to open it. Also, Niven is correct in that the groove you cut in the feedscrew will have to be wider than the part you are wanting the feedscrew to move, this is due to the angle of the helix. If your parts would move along the axis of the feedscrew tilted at the same angle as the helix you would use the exact profile, if you want your pats to set perpendicular to the top plane of the feed screw as you show then you will need to widen the groove. If your part were a sphere or ball, the groove could be the exact shape due to the single line contact, but the groove will have to be different if you are trying to put a cylinder thru.
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- feedscrew 2010.SLDPRT.zip427.1 KB
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Iain Hendry @ Matt Neuman on Jan 21, 2013 9:25 AM
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Hi Matt,

That's why I need to use a Solid Sweep Cut, not Profile Sweep Cut. Think about how Solid Sweep Cut works - it takes the solid, extended upward and downward, and would revolve it along the helical profile (from what the solid "sees", the screw is revolving around it just as it would as it feeds the parts along the conveyor). Profile Sweep Cut is the situation you're describing (which will not work, unless I "cheat" and just stretch the profile along the axis of rotation, which I don't want to do).

The part file you've included is close (close enough, really, for what I want to do) - but still isn't quite "perfect", it's still a bit of a compromise. It sounds like this "Cylinder only" thing is just a stupid limitation of the software... I guess there is no solution.

-Iain
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Niven Le @ Iain Hendry on Jan 21, 2013 7:39 PM
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Iain,
Solid Sweep Cut will not solve the problem. Even if it is possible, it would still yield the same result as profile sweep cut. Here is how you can prove it. Look at your "Part representation" solid, the one that is going to be swept, You can see that is is a straight slot. Now let's create a cyclinder out of that straight slot for testing the solid swept. This cyclinder has can match either with the right or left of the straight slot. Then you create a solid sweep cut feature using this cyclinder, and there will still be material left over; just like profile sweep cut.
I attached a file to show what I did.
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- Feedscrew 1.SLDPRT.zip794.2 KB
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Iain Hendry @ Niven Le on Jan 22, 2013 7:33 AM
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Okay, I see what you've done - I'm at a loss, then. For whatever reason, it doesn't accurately cut the profile, I guess. It leaves a very small slice of material left over.

Solid Sweep Cut provides a smaller error, but it's still wrong. It must be a SolidWorks glitch, then, because the logic in how the shape is produced is sound, isn't it?

-Iain
Attachments
- Solid Sweep Cut 2.SLDPRT.zip931.5 KB
- Profile Sweep Cut 2.SLDPRT.zip130.1 KB
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Josh Brady @ Iain Hendry on Jan 22, 2013 11:46 AM
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Here is the next question... Why do you want an accurate geometrical representation of the surface? Are you going to RP the thing? If not, I don't think you would want to try to fabricate it in any other way using the model.
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Iain Hendry @ Josh Brady on Jan 22, 2013 11:49 AM
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In this case, we outsource the part to a feedscrew manufacturer, who mill it on a 5-axis with a ballnose... watch the video I posted earlier in this thread for an example.

I want an accurate representation, because that's the whole point of machinery design!

-Iain
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Craig Hardman Jan 22, 2013 12:19 PM
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It's more involved, but why not do it like this?
It should get you more accurate geometry, no?
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- Feedscrew 1.SLDPRT.zip1.3 MB
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Iain Hendry @ Craig Hardman on Jan 22, 2013 12:22 PM
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Couldn't open your file... I get this error.

-Iain (SW 2012, SP5.0)
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Craig Hardman @ Iain Hendry on Jan 22, 2013 12:30 PM
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I saved it out using 2013, That is probably the cause.
Not being able to "down-save" files in SW is very annoying. Lol.
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Matt Neuman @ Iain Hendry on Jan 22, 2013 12:33 PM
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Iain,

If this part is being milled on a 5-axis machine, then Mark and Niven have both answered your question. There is no glitch in SW (as far as your part is concerned). Look at your part and feed screw from the side. Due to the "helix" of the groove, the groove has to be wider than your part because of the approximate 18 degree angle of the helix. Basically you are trying to make a 67mm wide part stand straight up in a 67mm wide groove that is leaned over at 18 degrees, it can't be done, the groove HAS to be made wider than your part so it has clearance at the top leading edge and at the bottom trailing edge. This is true no matter the shape of the part, whehter it is a cylinder, oval or square. You also need to change the shape of the groove because of the helical milling, the shape of the groove will never exactly match the cutter profile, this isn't a SW issue. The diameter of the cutter, offset from center and many other factors will determine the shape of the cutter.
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Iain Hendry @ Craig Hardman on Jan 22, 2013 12:35 PM
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Can you make a screenshot of SolidWorks (including the Feature Tree), so I can see your method?

-Iain
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Craig Hardman @ Iain Hendry on Jan 22, 2013 12:43 PM
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Pay attention to which sketch is highlighted.
You will still have some extra material as mentioned several times above, but it's one way to get around not being able to do the sweep with an slot.
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- ScrewFeeder.png412.8 KB
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Iain Hendry @ Matt Neuman on Jan 22, 2013 12:57 PM
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Your argument is valid for PROFILE Sweep Cut. Yes, if the 2-D Profile that is swept alonng the helix exactly matches the shape of the part, then sure - it won't fit, because of the tilt you describe.

However, SOLID Sweep Cut would remove material like this: The part is cut away from the screw... then rotated 0.000001 degrees or whatever along the helix, and cut again. And again, and again - which means that there should be zero material interference. But for whatever reason - even with our cylindrical simplification of what I'm trying to do - there's still an error, some very small amount of material left over.

-Iain
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Iain Hendry @ Craig Hardman on Jan 22, 2013 12:59 PM
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Thanks; that's a great workaround, and would produce geometry identical to what would be created if the oval could be Solid Sweept Cut along the helix in one step.

-Iain
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Craig Hardman @ Iain Hendry on Jan 22, 2013 1:04 PM
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It uses solid sweep to achieve it with the exception of the flat section that joins the two circles.

It's important to note that this will create the exact geomerty on the center plane of your part (See picture) but it will not create a perfect match the geometry you require.
The left over bit of material will just cause the "conveyed part" to be slightly tipped. This "normal" for these type of conveyor. Actually helps with conveying in some situations.
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- ScrewFeeder2.png182.2 KB
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Josh Brady @ Iain Hendry on Jan 22, 2013 1:33 PM
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"I want an accurate representation, because that's the whole point of machinery design!"

Umm, no.

The whole point of machinery design is to create a working machine. The drawings are only a tool toward that end. If adequate information is contained in a drawing for a machinist to create the working component, accurate graphical representation is not required. It is actually poor engineering practice to squander valuable engineering time in a purely aesthetic, intermediate step if it is not required for the manufacture of the part.
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Dan Bertschi Mar 26, 2013 9:50 AM
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Hi Iain & Everyone!

Not sure what has become of your design at this point, bu t I just encountered the same challenged. Simply, a cylindrical bottle to be moved by a variable helix feed screw. My customer was clear that the profile cut into the feed screw be a close match to the cylindrical bottle. I tried using the Solid Sweep tool without success.

Starting with 'round stock', I attempted to cut the groove with Solid Sweep. After encountering overlap issues, I cut the round stock in half, cut one body at a time, them combined. The results were still not acceptable. I discovered that cutter height, in relation to cutter diameter, and to stock diameter provides different results. None were acceptably creating a radiussed groove with cleared material to enable the bottle to stand upright.

It is NOT simply a matter of making the cutter larger to create the desired groove. Based on 'a circle through an angled plane creates an ellipse', I started with an ellipse, knowing I was creating a cutting angle with the helix. My solution used two normal profile sweep cuts, cutting half at a time to prevent overlap errors. The profile was defined with a partial ellipse and an angled line. I also create my profiles & start/end my helix beyond the ends of the feed screw to ensure a smooth entrance/exit of the cut.

If desired, I'll create some pics to post here.

Mark, I'm also going to contact my VAR and get a ball rolling to review this tool. It has great potential, and is needed. But, it must be able to accurately simulate the same results that a real tool & material would create in a mill/lathe. Unfortunately, it does not, it's close.
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Niven Le @ Dan Bertschi on Mar 27, 2013 1:41 AM
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Hi Dan,

Can you upload some pictures? This discussion really makes me scratching my head. I am one of those who see no problem with the features, and I would really like to see why some of us see it differently.

Also, if you can create a sample on Iain's file or your own file, that would greatly help.

Best regard.
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David Deaville Mar 28, 2013 5:03 AM
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Iain

I think this idea works. What do you think? I have made your original body into a revolved ring so that it can be used for a solid sweep cut.
Attachments
- Feedscrew 1 Rev2.SLDPRT.zip728.2 KB
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