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
TIA,
Timelord






RE: 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
http://www.EsoxRepublic.com-SolidWorks API VB programming help
RE: Swept solid
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
Jeff Mowry
www.industrialdesignhaus.com
Reality is no respecter of good intentions.
RE: Swept solid
mncad
RE: Swept solid
BTW, it sounds like an interesting problem. I'm tempted to ask for a swipe at it, but I'm swamped.
RE: Swept solid
Windows 2000 Professional / Microsoft Intellimouse Explorer
SolidWorks 2006 SP01.0 / SpaceBall 4000 FLX
Diet Coke with Lime / Dark Chocolate
Lava Lamp
RE: Swept solid
RE: Swept solid
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
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
Helpful SW websites every user should be aware of FAQ559-520
How to get answers to your SW questions FAQ559-1091
RE: Swept solid
Jeff Mowry
www.industrialdesignhaus.com
Reality is no respecter of good intentions.
RE: Swept solid
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 eager to see if it works properly.
Jeff Mowry
www.industrialdesignhaus.com
Reality is no respecter of good intentions.
RE: Swept solid
http://ww
Thanks for the FAQ CorBlimeyLimey
RE: Swept solid
Tutorial 5b
Is this what you mean to do?
RE: Swept solid
Helpful SW websites every user should be aware of FAQ559-520
How to get answers to your SW questions FAQ559-1091
RE: Swept solid
Fixed ;)
Stefan Hamminga
Mesken BV
2005 Certified SolidWorks Professional
Mechanical designer/AI student
RE: Swept solid
ht
This should be a bit more precise then the sheetmetal feature.
Stefan Hamminga
Mesken BV
2005 Certified SolidWorks Professional
Mechanical designer/AI student
RE: Swept solid
"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
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
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
Helpful SW websites every user should be aware of FAQ559-520
How to get answers to your SW questions FAQ559-1091
RE: Swept solid
As soon as I can figure out how!
Just tried pasting from screen shot,
didn't work.
Jeff
RE: Swept solid
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
Posting any files FAQ559-1177
Helpful SW websites every user should be aware of FAQ559-520
How to get answers to your SW questions FAQ559-1091
RE: Swept solid
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
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
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
"...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
h
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
http://w
Have a great weekend!
Scott in San Diego
RE: Swept solid
Helpful SW websites every user should be aware of FAQ559-520
How to get answers to your SW questions FAQ559-1091
How to post Images
RE: Swept solid
I looked at your track cam. I has a path that changes in width; no good as a cam. The cam follower will be loose in most of the track.
Timelord
RE: Swept solid
1)Organic body:
http://pu
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://pu
3)Complete your sweep, make sure its a seperate body
http://pu
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://pu
5) then copy the surface that was sliced away.
http://pu
6) Thicken cut....
http://pu
7) Completed slot....
http://pu
W.Y.T.D.N.T.Y Manual coming soon :)
"if you can't make it work...Cheat"
RE: Swept solid
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
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
" 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
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
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:/
I like messing with the limits of all software so I thought this was an interesting thread.
RFUS
Apple IIc
RE: Swept solid
RE: Swept solid
htt
RE: Swept solid
http:
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