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Swept solid
2

Swept solid

Swept solid

(OP)
I haven't loaded SW2006 yet, so I cannot test it but I was wondering if SW has added the ability to sweep a solid yet?  I tried to make a barrel cam once but couldn't get the slot so both sides remained tangent to my follower.  The only way I can see this being done is to have the ability to sweep the cylindrical shape of the end mill while translating and rotating the cylindrical cam blank.  The ability to sweep a solid has been requested of SW and promised since I can remember.  It seems to me that this should be a requirement of any decent solid modeler, otherwise it is near impossible to model a simple cut that any 2 axis computer controlled machine can easily make.

TIA,

Timelord

RE: Swept solid

I don't believe it does solids yet.  However, you can probably work around this by building the surfaces you need and then cutting with the surfaces.  (Depends what you need--I'm not sure what a barrel cam is or how it would require a swept solid.)

Yesterday I was able to complete some complex forms with surface fills and lofts--very nice in 2006.  Much less hassle with twisting and other complications and the results are great.


Jeff Mowry
www.industrialdesignhaus.com
Reality is no respecter of good intentions.

RE: Swept solid

Swept solids is on the bleeding edge of mathematical theory, far from mainstream CAD application programming.  Don't expect to see it in SW or anywhere else before someone wins a Nobel prize for it.

I could be the world's greatest underachiever, if I could just learn to apply myself.
http://www.EsoxRepublic.com-SolidWorks API VB programming help

RE: Swept solid

(OP)
Theophilus,

Thanks for the quick answer.  It is not possible to work around this limitation, I've tried many different ways.  The line guide cam on a fishing reel is a type of barrel cam.

TheTick,

I can't be all that bleeding edge, the software that calculates tool paths for NC machines must do it all the time.

Timelord

RE: Swept solid

So is the difficulty in keeping the orientation of your solid "tool" aligned the way you need it with the part and path?  I think this could be done by sweeping a profile in the example you gave above, couldn't it?  Couldn't this be done with guide paths?


Jeff Mowry
www.industrialdesignhaus.com
Reality is no respecter of good intentions.

RE: Swept solid

I have requested the same thing from SW.  I did get an email from them earlier this summer showing a sample of a swept volume, but it was somewhat limited.  I have no idea when they are looking at adding it to the software, it is not in SW2006 yet.  Not having that capability is somewhat of a limitation for us also.  We can't model our parts to look like what is actually made on the shop floor.  The parts are close, but not exact and it takes alot of effort just to get them close.  Hopefully it will be added soon.

mncad

RE: Swept solid

CNC software is actually sweeping the 2D cutter profile, not the full 3D shape.  (The sweep also accounts for the 180° zero radius end of a cutter path).

BTW, it sounds like an interesting problem.  I'm tempted to ask for a swipe at it, but I'm swamped.

RE: Swept solid

I'd love to swipe at it... but I got no clue what you're talking about


Windows 2000 Professional / Microsoft Intellimouse Explorer
SolidWorks 2006 SP01.0 / SpaceBall 4000 FLX
Diet Coke with Lime / Dark Chocolate
Lava Lamp

RE: Swept solid

I'm referring to the barrel cam follower referred to in the original post.

RE: Swept solid

2
The only way I have come up with to model a track cam is to do it with sheet metal.  It is a bit of a hack but it produces quite good results.

Basically you model a sheet metal tube, unfold it, cut the cam curve out of it and then refold it back into a tube.  You can then extrude a cylinder inside it to make the body of the cam.

SW sheet metal functionality makes sure that all edges of a sheet metal part remain perpendicular to the face of the sheet.  This is same thing that happens when you machine a slot in the periphery of a cylinder using a cylindrical cutter who's axis is perpendicular to and intersects the axis of the part being machined.

To get a closed track I have to make two parts and put them together in an assembly to get what I want.  I guess they then could be joined but I dont bother.

I could offer an example part which would describe the process better than I can here in words.  The process is really pretty simple.

If one of you guys with a website would be so kind as to host it I could e-mail the parts and an assembly.

Tom Rice

RE: Swept solid

... now I get it!

Thanks Tar


Windows 2000 Professional / Microsoft Intellimouse Explorer
SolidWorks 2006 SP01.0 / SpaceBall 4000 FLX
Diet Coke with Lime / Dark Chocolate
Lava Lamp

RE: Swept solid

You can also do a similar process with surfaces--then thicken the surface to keep the edges perpendicular to the outer surfaces--but the sheetmetal trick takes some hassle out of it--nice hack.


Jeff Mowry
www.industrialdesignhaus.com
Reality is no respecter of good intentions.

RE: Swept solid

Shoot Theo... I was just going to try that... It should work though, I think.


Windows 2000 Professional / Microsoft Intellimouse Explorer
SolidWorks 2006 SP01.0 / SpaceBall 4000 FLX
Diet Coke with Lime / Dark Chocolate
Lava Lamp

RE: Swept solid

Be my guest--I don't have time to try right now anyway. ..

I'm eager to see if it works properly.


Jeff Mowry
www.industrialdesignhaus.com
Reality is no respecter of good intentions.

RE: Swept solid

tar ... it looks like you cannot have spaces in the file name.


Helpful SW websites every user should be aware of FAQ559-520
How to get answers to your SW questions  FAQ559-1091

RE: Swept solid

tar writes:

"SW sheet metal functionality makes sure that all edges of a sheet metal part remain perpendicular to the face of the sheet.  This is same thing that happens when you machine a slot in the periphery of a cylinder using a cylindrical cutter who's axis is perpendicular to and intersects the axis of the part being machined."

No disrespect, but I think this only holds true if your cylindrical cutter has a diameter of zero. As soon as your cutter has a real diameter, the walls that it cuts are parallel to the axis of the cutter, which is perpendicular to the surface on where the axis of the cutter intersects the surface.

I have solved a similar problem where I was trying to cut a male threadlike form for a camlock (sometimes called a bayonet lock) mechanism by creating a sketch on a face parallel to the axis of the cylinder above the surface and then doing a wrap onto the surface. In other words, create a cylinder that is the "minor diameter" of your cam, then wrap the sketch feature onto it with the thickness of the wrap defining your final "major diameter".

It is a bit tricky if you need the opposite edges of your sketch to connect once wrapped, but it does work.

Scott in San Diego

RE: Swept solid

Scott - take a look at the link Jabberwocky posted.  Professor Mather has a great resource for examples and freely shares his tutorials.  I had a bayonet feature I had to put into a part which really taxed my MCAD abilities....lucky for me I was doing this in Pro/E 2001 and had a different tool box to pull this off.  I used the graph function and Trajpar for those that know Pro/E....did it all in surfaces then did a transform since this feature was part of three around a cyclinder.  Anyway, a little of topic.....I worked through that tutorial 5B and it's the way I would do a cam since you can define the profile on that sketch.

Best Regards,

Heckler
Sr. Mechanical Engineer
SW2005 SP 5.0 & Pro/E 2001
Dell Precision 370
P4 3.6 GHz, 1GB RAM
XP Pro SP2.0
NIVIDA Quadro FX 1400
      o
  _`\(,_
(_)/ (_)

"Coming together is a beginning, staying together is progress, and working together is success." - Henry Ford



 

RE: Swept solid

Timelord,

I just created a Planar Surface from a circular sketch, then created a sketch path line & arc, then did a sweep from the sketch circle (not the planar feature) and created a swept solid. Easy. Nobel Prize please.  :)

Jeff

RE: Swept solid

Can you post an image or file please?


Helpful SW websites every user should be aware of FAQ559-520
How to get answers to your SW questions  FAQ559-1091

RE: Swept solid

CorBlimeyLimey

As soon as I can figure out how!
Just tried pasting from screen shot,
didn't work.

Jeff

RE: Swept solid

Heckler,

Thanks for encourageing me to look at Prof. Mather's examples. Some great stuff in there.

I started out similar to Mather's example 5B, except my sketch plane was an offset from the tangent plane to an arbitrary distance above my cylinder. I then used "emboss" instead of "deboss". I just played with my sketch until this generated the geometry I needed directly. I don't understand why Mather's example bothers with converting to surfaces and stitching and stuff. Seems to add some unnecassary steps, but I may be missing something. My profile has different geometry for the top and bottom cam surfaces.

Scott in San Diego

RE: Swept solid

CBL, TL,

Perhaps what Timelord is requesting and what I read from
his post are two different things. I just created a common sweep of a planar sketch. It is a solid, it is a sweep. Am I missing something?

Jeff

RE: Swept solid

yanceman,

I believe everyone here is talking about creating a solid (cylinder to represent a milling cutter) and then creating a cut that follows a path (helical most likely) with that solid cylinder.  This is not possible to do or replicate (easily) with SW.  

mncad

RE: Swept solid

Mncad,

Ahh. Well, I know you cannot create an extruded feature, then sweep that solid feature. At the same time, an end mill will have a square profile, and this cut can be duplicated in a cut-sweep, as long as the sketch remains perpendicular to the helix path (like the lands and grooves of a gun barrel).

Jeff

RE: Swept solid

Yanceman said,

"...and this cut can be duplicated in a cut-sweep, as long as the sketch remains perpendicular to the helix path..."

There in lies the trick. In my experience SolidWorks is not very good at keeping the sketch perpendicular to the helical path, even with helical guide curves. Even if it was, this method won't work very well if need your sweep path to have any non-helical geometery like any kind of bumps or indents in the cam surface. The wrap works much better, becuase you have a 2D sketch were you can define your cam geometry and also something to put on the drawing when it is time to actually cut metal.

Scott in San Diego

RE: Swept solid

Here is a link to a part I created in Pro/E using Trajpar and the Graph function.   The bayonet cut was made entirely of surfaces and knitted together....this was a real head scratcher.  In total it took 15 features to create.  A simple part if made on a 5 axis mill.

http://www.mooload.com/file.php?file=files/1130535151/v31603-d-1.SLDPRT

Anyway, I'm not trying to start a my MCAD is better than yours statement.  I done equally complexed stuff in SWx that would be a real pain in Pro/e....ie draft features.  Draft is a real pain in Pro/e.

Best Regards,

Heckler
Sr. Mechanical Engineer
SW2005 SP 5.0 & Pro/E 2001
Dell Precision 370
P4 3.6 GHz, 1GB RAM
XP Pro SP2.0
NIVIDA Quadro FX 1400
      o
  _`\(,_
(_)/ (_)

"Coming together is a beginning, staying together is progress, and working together is success." - Henry Ford



 

RE: Swept solid

How to approach it along a extremely organic surface......

1)Organic body:

http://putfile.com/pic.php?pic=11/30410014389.gif&s=x11

2)Set up sweep, notice that the path is COS, it will only work when the Curve is on srf, and always use a circle as your profile.

http://putfile.com/pic.php?pic=11/30410020290.gif&s=x11

3)Complete your sweep, make sure its a seperate body

http://putfile.com/pic.php?pic=11/30410021915.gif&s=x11

4)Use the face of the orgainc surface to do a cut with surface to slice away the sweep, so it looks something like this....

http://putfile.com/pic.php?pic=11/30410032151.gif&s=x11

5) then copy the surface that was sliced away.

http://putfile.com/pic.php?pic=11/30410034173.gif&s=x11

6) Thicken cut....

http://putfile.com/pic.php?pic=11/30410053186.gif&s=x11

7) Completed slot....

http://putfile.com/pic.php?pic=11/30410064789.gif&s=x11





W.Y.T.D.N.T.Y Manual coming soon :)

"if you can't make it work...Cheat"

RE: Swept solid

Timelord,

I was only trying to share with you a technique to get over a modeling problem that you by your own admission could not crack.

I spent maybe 20 minutes on the parts and didn't bother to work out all the details or even define the sketches involved.  There's 20 minutes of my life trying to help you out that I will never get back.  

Won't do that again.

RE: Swept solid

(OP)
tar,

Sorry you wasted your time.  I did not say that I couldn't crack the problem.  In my original post I said "near impossible" meaning I have worked around the issue, but like you I don't like to waste time especially when it is working around dumb limitations of a software package.  I will reiterate, the ability to sweep solids should in any basic solid modeler, because that is how parts are really made.  The cam example is just one place where the limitations of 2D sweeps and extrusions becomes obvious.

Timelord

P.S.  Your method is not the one that worked for me, it has problems you have yet to discover.

RE: Swept solid

In your subsequent post you said:

 " It is not possible to work around this limitation, I've tried many different ways."

My way is the only way I've found using SW2003 which is where I'm stuck at the moment.

It's really just a matter of visual representation anyway.  If I'm making a barrel cam I'll spec the cam curve and program the part to that.

RE: Swept solid

Timelord,

Did you try the method in Prof. Mather's example 5B as referenced by Heckler and discussed by Heckler and myself? Did you look at the parts posted by Heckler and myself? Do they accomplish what you are trying to do or are they two different problems?

Thanks,

Scott

RE: Swept solid

In 2006 you can create a curve driven pattern and align the solid body(s) in the pattern tangent to to a curve, where you select a face normal to align the body. This face normal can be a swept surface created from a line on a helix for example. You can then cut the solid body to create a profile and the generate a pattern with a high number of instances and equal spacing using this method. A loft or lofted cut can then be generated by just selecting the faces, no sketches, and just use connecters due to the high number of faces in the pattern, otherwise you'll need a lot of guide curves. This, I find, is a great way to make lofts, and is the closest way I can think of to loft a solid, because you can go to each solid body in the instance, be it 5 or 1000 and create the profile you want with a specific profile cut for that body. I hope in the future you can create a loft the same way a curve driven pattern can be created.

If you wanted to create a finely faceted swept solid it can be done. It just depends on you mean your rig for SW is. Plus, in the postprocessor world, G1 contoller moves always boil down to absolute or incremental moves, and G2 and G3 are interpolations of precise geometry.   

If a solid body was patterend a very large number of times with a very small spacing between each one, lets say like .0005 (the accuracy of a controller, at least mine), and then all these bodies were combined, you'd have a close to a swept solid. I tried this with the pattern technique above and did 2000 instances with .001 spacing. I could not get them all to combine at onece and got three different error messages with each attempt to combine, but by doing a few at a time I was able to create something similar to a swept solid. I then was able to use this with the subtract and indent (cut) function.
  
Here is an example of what I am talking about. See the black and gray tool lookin thing far left. Thats 40 bodies combined into one. You could get pretty extreme with this. The other shots are what I mentioned in the first paragraph of this long post.


Here is a 2006 file of whats seen above. How many instances can you create with the first curve driven pattern.
http://www.mooload.com/file.php?file=files/1131576832/SweptSolid_ayuh.SLDPRT

I like messing with the limits of all software so I thought this was an interesting thread.

RFUS
Apple IIc


RE: Swept solid

Here is the image, grabbed the wrong size

RE: Swept solid

Doesn't help us Solidworks users at the moment, but the Swept Volume Envelopes has been available in Pro/E Mechanism for many years now (no Nobel Prize winner referenced) and you can follow the link below to see an animation of it.
http://www.ptc.com/products/proe/animations/tire.htmand

Now that Pro/E has been repriced in the Solidworks range, it is a quite compelling option for high end, low cost CAD.

The feature has also been in CATIA V5 DMU kinematic product for several years now as well

RE: Swept solid

Is it a true swept solid or an approximation?

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