Thank you so much. It's your youtube video that I posted asking if someone knew how to make the drawings.
Great help to get it from you.
Just a quick question, how did you make the pins rotate? What relationships did you use?
I'd like to share my experience. Solid sweep cut is good command, but it is very sensitive for the path and the "tool" geometry. If you use a "ball nose milling tool" it will give a very fast solution and after this you can edit the bottom of the slot... Using simple path gives better results.
Here is a video:
I hope, this helps and have a nice weekend my friends!
I will immedeatly go to test wether with SE2019 wrapped curves can be used for Solid Sweeping, as seen in Your video.
EDIT: Hi @Imics Your method is working with SE2019 in a range of geometric situations, but I have seen, that if the angle between the path lines gets to sharp the Solid Sweep fails.
But it is better than it was ever!
what I wanted to say is, that there could be geometric situations, where the Solid Sweep will not work at all.
See attached video, where - as long as the tool itself is not to long, or does not go to deep into the shaft - the Solid Sweep is created, but if You enlarge the tool it fails.
I have run into that situation, as I started the sketch in a different/wrong way as "N" shape and not as You did.
So I have very sharp edges between the radial path and the guiding path.
And this seems to make problems, although I can not understand or see where they could be.
But the are there somehow.
But anyway, this is better as assumed or as it was, when this feature was introduced.
I believe, that there were no possiblity to use the wrapped curve at all, even with a ball nosed end
In ASM I use the ASM path relationship and a rotatal motor to make the
video. Additional relationships are needed to control the pin position
and keep it from flipping.
You should be able to see these in the zip of the ASM I uploaded.
what also is surprising me somehow, that if the shaft itself is a "thinwall cylinder" (pipe) and the tool is going through the wall, that then also the length of the tool has influence wether or not the Solid Sweep is created.
Same is true for the shape of that tool.
Changing the ball end tool to a flat end tool, what IMHO may not change anything for the resulting sweep, lets the feature fail.
This all together shows, that the Solid Swepp functionality is depending very deep onto the situation and definition parameters, and this always is a very critical issue for a user, that sometimes the feature is working where in other situations it does not.
PS.: also changing the radius from 5mm to 5.2mm lets the Sweep crash!
Again, something I can not explain why, what might be the reason.
every solutios from others are exeptional!
However, I would like to ask any of you, if there is a better way (or will be in next SE release), how to create Solid Sweep using wrapped radius trajectory?
I already create PR year ago, so anyone is welcome to join me :-)
PR8954376 (ability to continuously orient the tool perpendicular to a cylindrical surface)
Gentlemen, thank you so much for your valuable input.
Sorry for being a bit silent, I've been out of the interweb doing some installation work
Based on what is available now, ie - SE 2019, what do you think is the most suitable method to get a realistic CAD model we can manufacture ? Anyone built cams such as this for work before?
I spoke to our machinist who's highly experienced and he told me he can produce a cam if I give him the following info -
PCD of followers
Diameter of follower
Number of followers
Of course things like load, indexing angle. dwell angle will have to be given as well.
But basically, bigger the arc of the followers, the bigger the barrel can be which will make lesser of a ramp on the cam etc. Also means we can use bigger bearings as well.
I've attached the latest model of our attempt to draw a barrel cam as well. But again, manufacturability is where I'm concerned.
Looking forward to your input.