SolidWorks - Barrel cam design
I designed a barrel cam for an automated machine that is straight cut along 180 degrees of rotation, then a helix along 60 degrees of rotation pulling a cam follower back 2 inches, then straight again for 60 degrees, then a 90 degree turn back to the first path.
After some futzing I figured out how to model it - now I am having a devil of a time getting a cam follower to mate to the surfaces.
I have tried tangent mates, path mates, etc. with marginal results. (the model locks up tight in places or jumps around rather than smoothly rotating).
Anyone here have experience with barrel cams and animating a cam follower to follow the cam? I would like to animate the linkage design for a customer presentation and the process of defining a mate to geometric surfaces works fine - but the helix portion causes the model to puke.
I'm afraid my brain is too scrambled to follow the textual descriptions - I only add up to 300 degrees? (Or 390 if I'm totally off somehow). Do you have the model itself? (Or rather, can I have a look? PM possibly?)
(Is the surface you want to follow a single closed continuous surface? Unless you had that in mind when modelling I guess chances are that the cam part consists of several surfaces, and that would be an issue. I'm thinking a rebuild to a single surface to follow might be worth a try).
I ran into the same kind of problem. Seems what was messing things up was the transition between surfaces of the curves.
The cam (depending on what Mates were used) would follow one section or profile, then would not follow the next.
However, I did get a Pin to follow a Wrap-Cut from a Sketch that was made on the Top plane; and that provided a smooth action as the "barrel" was turned.
Not sure if tangency lines cause a problem using this method....worked on this sample tho'.
You might also search for Cams on YouTube SolidWorks tutorials
SolidWorks 3D CAD products - Swept solid
These guys are discussing "swept solids", and the examples given sound like your challenge.
They say Solid Works isn't up to the task.
If the WrapCut is used, the dimension in the Sketch for the 360deg must be a function of the circumference of the "barrel"
You might try doing a 3D sketch and then attaching your part to follow the sketch instead of the surface.
I created the path using a 3D sketch - using a combination of arcs, lines and a helix. (rather than using a wrapped sketch) It is the joining together of these elements to create a path that has been the challenge. This sketch is along the exact center of the path. I used the profile sweep along the arcs and lines and I used the solid sweep along the helix keeping the solid normal to the surface. The cam from a modeling standpoint is in good shape dimensionally and functionally.
The helix starts and ends at the exact dimensional locations of the other line segments, but because it is a helix, it is not possible to connect it to the line segments to create a continuous path. I would really like to nail this for a presentation next week. It has been driving me batty for a couple of days now.
I assume that the surface you are trying to follow is actually made up of multiple smaller surfaces. It may help to join the surfaces with a knit (Insert-> Surface ->Knit) so that it sees it as one entity in the assembly.
Anything made out of arcs and lines will make separate surfaces even if wrapped. Rebuild as spline and then you'll be talking. Knitting surfaces wont help either - it will just group them and signify that the connections are tight when making solids.
To make a single surface going all the way around you need to use splines/ NURBS.
1. First round off any sharp corners ever so slightly.
2. Duplicate the inner (or outer) edge to make a continous line around.
3. Rebuild that line as a tight fitting spline.
4. Build a surface radial from that single line. (Dont build two lines from both outer and inner edge in order to sweep - number of control points might be off and likely also be placed differently). Extend surface both ways and cut edges from above just in case there are some spline innaccuracies in zx plane. (Or project spline to sylinder before making the surface).
5. Use replace surface function, split and knit or otherwise exchange the previous surfaces with this single surface.
Or use wrap and a spline directly from there.
If this fails export part to Rhinoceros, make the surface, and import it into Solidworks.
I must admit - I am a bit of a hack in Solidworks and have been at it part time for only about 6 weeks. . . I'll see if I can follow your instructions and achieve the desired results.
If worst come to show just send me that thing and I'll go all Rhino on its ass.
Wrap and spline seems like the easiest approach in Solidworks though. I think there might even be a CAM wizard hidden there somewhere.
Law Curve Using Expressions In SW
I was involved with a very similar problem using NX not SW:
Originally Posted by motion guru
If you look at a certain American made machine tool's wheel style tool changer you'll see a variable helix barrel cam. That cam is produced using a mathematical expression to drive the curve. Two problems arose (as explained to me from the designer) that I think you're dealing with.
First - using SW, the designer could never get the two sides of the slot for the follower to remain perp/parallel in it's entirety (which causes the binding). At the time, SW could not interpret expressions to create splines. So, they found a math wiz who would convert the math expression straight to a centerline only nc toolpath for the part to be produced.
This created the second problem:
Custom diameter end mills had to be used to cut only center-line in the slot. This meant only fresh tools (no regrinds) could be used. This was a $75,000 yr cost in tools.
They ended up getting NX after being shown Law Curves that could read the expressions properly to create the splines. At that point they could also machine the barrel using re-ground tools as now you have two splines to drive intead of just down the center.
Don't know if that helps but that's how that went down... : )
Turns out Solidworks wont accept a spline/NURBS surface as a mate even though it is a (ruled) single continous surface. So much for that theory. I guess the path and tangent mates will have to do then.
What versions of SW are involved?
The thread on eng S_W_Bausche refered to are dated 2005. There have been 4 or 5 upgrades since then...
Same w.r.t. BillT's observation - it's easy to believe that some prior version of SW couldn't do the task so people went to NX (or Catia?)
But is that true of the current version? (And does Motion Guru have that version.)
There is a solidworks forum which I've found helpful in the past, you might try posting the same question there.
(You do need to register with their porthole...)
I am on SW10 latest revision - I have come to the conclusion that while you can accurately define the geometry within solid works - you cannot mate a cam to the surface to animate the assembly.
A tangent mate works fine for the cam until you get to corners, a path mate works fine as long as the path is continuous - for whatever reason - SolidWorks cannot create a continuous path without dorking up the Tangent nature of the surface relative to the cam follower (thus blowing the tangent mate up at various locations) and SolidWorks will not allow the use of a spline to define a cam path using the cam mate.
One additional challenge with this model is that the cam is on a 4 bar linkage and while I have the geometry correct with the cam follower centerline orthogonal to the axis of cam rotation - the cam follower plunge depth in the groove does vary with the rotation of the linkages.
BadBeta provided a continuous surface that mimicked the cam - even this does not serve as a suitable mate / path definition within solidworks.
I spent a few hours on various SolidWorks forums prior to posting here - at present, I am going to animate a portion of the travel at a time by suppressing / unsuppressing mates and using the motor function to rotate the cam.
I'll check out that link to see if there is anything there that I haven't already read - but for now, I think I will use the tedious method of stitching together short segments of animation based on the various mates that work for different segments of the cam into a seamless video.
Not sure if you can use it with the added complications, but for others reading this there is a free "barrel cam and follower" Solidworks sample setup at Camnetics. Worth looking at.
Camnetics :: Freebies
I've had to do the same thing recently, here is what I did, maybe it can help.
First, create the barrel, then a plane tangent to the barrel. Make the cam profile on the tangent plane, following the advice earlier to ensure there are radii on all of the corners of the cam profile. Use the wrap feature to wrap the cam profile onto the barrel. This is configuration 1.
Create a 2nd configuration of the cam (or copy the cam under a new name). On the 2nd config, boss extrude the cam profile on the tangent plane, to any thickness.
Insert the 2nd config into the assembly, mate it using planes such that it can slide sideways. You may want to use a limit mate here. Then, mate the follower to the flat cam on the 2nd config. Finally, mate the 1st config barrel cam to the 2nd config cam using a rack and pinion mate, and align the starting positions of both so that they match. When the barrel is moved, the rack and pinion mate drives the 2nd config flat pattern cam, which drives the cam follower. Hide the 2nd config, and it looks like the barrel cam is driving the cam follower.
I have done similar things with 3d sketches in the driving part and a sketch point or ref point in the driven part. Mate them together with a simple coincident mate in the assembly and control the rest of the movements of the driven part with additional mates between axis and planes. Not sure if you can make it work but its another way to look at it.
In the case where I used it I had an inner sleeve with a cam sticking out of it thru an outer sleeve with a cam slot. when the inner extended it rotated based on the cam slot. I drove the inner with a limit mate and the rotate with a two sketches as described above. It worked slick but it only rotated 180 and I didnt "drive" it either
the best way to mate followers to barrel cams is to create your follower path using a continuous curve and then mate a point on the follower coincident to the path. the curve data i bring in as a "curve through xyz point" generated in excel or mathcad. the key is to use the curve for the mate, not the surface.
i've done it quite a few times with good success.
I ended up getting it to work in an animation using keys to suppress mates at various locations and form new mates.
One section of this cam is parallel to the axis of rotation - and is intended to be at that location during dwell and is actuated with a pneumatic cylinder. As such, it is impossible to get a mate to follow that surface while the cam follower is being driven through a series of angles.
Now for an hour or two of camtasia (not related to cams) and it will be ready to send to the customer for review. Thanks to all for the comments - and BadBeta thanks for taking the time to look at my model and take a whack at the surface challenge.
On to the next stage . . .