If I try to cut a part in 4 axis where the surface dips below the centre of rotation BobCad/Cam ignores that area and leaves lumps of stock.
I’ve tried translating the part and have proven that lifting it above the centre of rotation will solve the issue, but only on one side as the part has low sections 180 degrees apart so
it’s impossible to have both above centre.
Attached are screenshots of part with paths and sim showing stock left where the part dips below centre line.
Circular and helical paths leave stock in the same places.
Is this a known limitation?
Is there a solution?
All suggestions welcome,
It fails on a really basic single throw crank too –
A very kind chap on cnczone helped out on the issue of rotary cuts below the rotary axis.
Although the somewhat cryptic Help entry gives no hint of this it’s the Base Point which needs to be set to define a base axis within the part independent of the rotary axis, paths can then be generated down to this Base Point. (Base Point isn’t even a point, it’s an alternate axis for the part parallel to the defined rotary axis.)
If your rotary axis is in X then use Y and Z to define an alternate Base Point axis parallel to the rotary axis and use this just to generate paths for the problem section.
Parts with multiple sections where one axis will not suffice can be processed as several sections, each with it’s own appropriately set Base Point (It’s not a point it’s an axis).
For my S shaped part I needed 3 Base Points with the job split into sections along the axis, see image attached
Close inspection of the paths on the thin end of my part reveals them to have a slight “figure eight” distortion which I’ve been unable to resolve with any of the settings available in the rotary feature
It’s been a while and it would be nice if it worked and/or feedback was forthcoming.
Rotary was a feature in the flyer for 4-Axis Standard, crippling limitations were not mentioned.
Forth Axis Standard / Rotary :
The problem that I am having is to use it for roughing or finishing with multiple passes which are offered as options in the Feature menu / Parameters is that the distances seem to be so minimal between the upper and lower surfaces that you get an area of rapid tool path if there is to much space between them. It is very time consuming to get tool path to work. Heck I wouldn’t even be able to make Pinocchio’s mug after he has told a few small lies without a lot of extra programing.
Am I doing something wrong?
If there is and easier way any help would be much appreciated.
I prefer to use zig to keep thrust in one direction on rotary.
Nothing like over the Hills and through the Woods to grandmothers house we go, and she just lives next door.
Now we have some answers on CNC Zone, so far it’s what had already been suggested or worked out and posted on CNC Zone.
1. Don’t rough Rotary, Rough 3-Axis with indexing (as it’s faster and more efficient) leaving enough material (not much though) for the “Roughing Pass(es)” in Rotary which are there purely to allow the removal of excess stock left after 3-Axis Indexed Roughing.
2. Base Point defines an offset axis (which the software uses as a base point from which to calculate it’s cutting paths – the name makes sense once you know what it does, this really should have had a far better explanation in “Help”) to be used with a defined length of the job that is off centre from the rotary axis, dividing the job into multiple sections with different Base Points is required for parts with multiple offset sections.
For anyone not familiar with CNC Zone Al’s thread where he’s covering Rotary in Standard can be found here
I wish this wouldn’t be also an issue that I would face when I am doing my copy. This is the reason why I am now doing plenty of research to make things better without glitch or whatsoever concern that will arise. Thankful I am too that I have colleagues working from http://digitekprinting.com/ that also have knowledge about this…
You must be logged in to reply to this topic.