respected Giulio fraulini..thanks for ur concern over my problem...i waiting ur tutorial....and also which software u r practical with???
Remaining in PTC ambit, I am practical with MathCad 15 and Creo 2; but I don't understand this what has to do with the main argument.
Thank you for the video, Giulio.
I have a question regarding the cylindrical cutting too. How are you accounting for the difference?
Maybe I missed it in the video, but I am trying to understand alternatives to pattering the cutting tool.
Asif, generating the desired motion profile is a separate discussion.
There are several ways this can be done based on a simple x-y graph of the desired profile.
Profiles that use sinusoidal profiles are easier to program.
I suspect there is a problem with your measurement analysis for clearance. If you are checking clearance in the same locations as the trace curve, then yes, you will have zero clearance. If you check clearance globally (collision), you will see this before and after the current position. This is what I was trying to show you in the 3rd post.
Along the radial position, this is not an issue. Only along the z-movement (helical movement) of the rollers is where this becomes prevalent. This is easy to check. In the groove, Create an axis between the 1st two trace curves at ratio 0.5. create a plane and revolve cut of what would be your roller bearing profile (including depth). You will find that there is material being cut with this operation, before and after the position of the measurement done with the analysis.
I only say this because in practice, if the part is being machined using a cutter the same diameter as the bearing (with clearance of course), this anomaly would be averted due to the motion of the mill and lathe. But if the is done with a cutter that is smaller with a number of passes, and you are concerned with minimal and consistent clearances, you will have to account for this. If the parts will be processed using a rapid prototype method where conventional tooling is not used, your cam will bind.
Generally, the sweep method and the boundary blends will generate the same profiles. You actually only need two trace curves for the sweep. You can compensate for the issue I raise with making the cut deeper (obviously) and wider to make sure that cut with the patterned cuts is fully cleared. If you want to make sure that your model is 100% accurate, and you want to manage a minimal clearance along the entire path, you have a lot more work to do. With a sweep profile, you can make a variable sweep that follows additional curves. created from known points along the path. These are the points where the patterned revolve cuts removed material.
-Most- of us do not need to be concerned with this as learned craftsman already know about this phenomena. But if you have to analyze a failure or some unexpected anomaly when you build your parts, maybe this discussion will give you some insight as to what might have happened.
Asif, this may help a little in defining motion with custom servo motion rather than tables...
and some more here... see the WF 2 link in comments...
For anyone interested, I attached a Creo 2.0 version of the video file. Just run the mechanism analysis to get the motion and play with the motion profiles and such. The drive servo motor is the default 10 second ramp and the driven motor is user defined for the 8 seconds of dwell and 2 seconds of motion (cosine*180).
I simplified the sweep by using thicken with center offset from a surface ribbon following 3 trace curves.
I did not do a lot with the interference issue here other than to provide some feature to either minimize it or just have a default clearance to account for it. Again, if you tell a machine shop the motion you need, they know what to do with that.
The idea of this part is that if you were to 3D print it, it would function.
I check clearance between parts, and not in the same locations as the trace curve.
In "partial collision detection" check in playback tab, inside mechanism environment, nothing enter into collision.
I attached a pdf file that explains the question.
Also the measure feature checks that there aren't compenetration (as I showed in the video into the ppt file). Naturally, you have to stare that inside mechanism, where it does the verification over all the time.
Interesting, it's like a 90deg version of a Geneva drive.....
Unfortunately, we cannot do solid-body sweeps. That is ONE big area where Solidworks actually has an advantage. This capability is LONG overdue. PTC, are you listening????
Interesting. I will have to review this. I am finding all kinds of deviations depending on the method used.
Thanks for posting.