Cancel
Showing results for
Did you mean:
Highlighted

Pioneer

I was pointed out today at the limitation of our controller in measures of lines per minute/second executable.
So my thought was to try and grasp how the relation could be of path tolerances and amount of lines of NC code.

Theoretical example:
- I can drive up to 60m/min my axis,
- and up to 0.5ms /line of code.
> so I can only program 120 000 lines of code /min,
> so per line I can take steps of min. 0.5 mm per line?

When I enter a intol and outtol of 0.001mm , would that not produce on a freefrom surface too much lines of code to be running at full feed?
Ofcourse this situation is a bit extreme, I haven't been anywhere near this point.
But is the thought behind it correct?
What would be the expectable relation between intol and outtol values and the lines of code for general freeform milling?

9 REPLIES 9

# Re: Relation 'intol outtol' and CNC code lines for freefrom machining

Gears Esteemed Contributor

Pretty simple:

The tighter the tolerance, the more lines of code ;-)

If you are looking for an equation, that is much harder, as it is surface dependant.  A smooth, "large radius" surface will need fewer points than a wavy, "small" radius surface.  I would suspect for a given surface, you can develop "rules of thumb", but if those rules are usable on other surfaces.  And I would guess they are non-linear.

I'm not sure if you can analyze the internal toolpath for distance of each move (I think you can, but I'm not sure), but you can definitely do this in the post (although that may 'break" turbo mode, assuming you use turbo mode in your post).

Ken Akerboom Sr CAx Systems Engr, Moog, Inc.
Production: NX10.0.3.5 MP16/TC11.2
I'd rather be e-steamed than e-diseaseled

# Re: Relation 'intol outtol' and CNC code lines for freefrom machining

Pioneer
I will give it a try and see how my example file results, I'll put some feedback here, for being complete.

I did not hear yet from the Turbo Mode, but it sure sounds as something I want to investigate too.

# Re: Relation 'intol outtol' and CNC code lines for freefrom machining

Phenom

@Michiel2, this is not a simple question. But in theory you are correct. However, most of the time you don't need to tighten the tolerance too far. Instead, activate one of the high speed modes on your machine, give it enough points to represent your surface, and let it smooth out whatever happens between the points. Assuming your contours are smooth the machine's algorithms will do a nice job of point fitting and smoothing. If your machine supports NURBS, this might be an even better way to go. Most machines will have different flavours of smoothing, some optimizing accuracy, others smoothness or speed.

Harri

# Re: Relation 'intol outtol' and CNC code lines for freefrom machining

Pioneer
I've did the test on a small contour operation.
NC code is 3676 lines when intol/outtol is set to 0.100
NC code is 30535 lines when intol/outtol is set to 0.001
But I noticed a limitation in our post we need to improve before we would ever reach the limit of our machine.

As far as I understood @hjoy the need for 0.001 would be very low, so looking at the difference in lines, that will save us also a lot of abundant code lines.

# Re: Relation 'intol outtol' and CNC code lines for freefrom machining

Phenom

@Michiel2, you might need something in the range of 0.001 for close mold work, but that's about it. Unless I'm doing optics I rarely go below 0.003mm in/outtol. I've understood that NX will put the line end points on the actual surface and let the connecting chords differ according to the specified tolerance. This means that the end points will always be as true to the surface as possible. But this is info that will be hard to find in print. Think I picked it up in one of Alexander Freunds posts regarding high quality surface machining a while ago.

Harri

# Re: Relation 'intol outtol' and CNC code lines for freefrom machining

Phenom

One afterthought which you are probably aware of:

When roughing/semi-roughing or even semi-finishing you'll always be leaving some material, so tight tolerance isn't necessary, it just slows toolpath generation and bogs up the controller. When finishing, I'm pretty sure you are not going to be maxing out the feed. 60m/min would require some serious spindle RPM for any reasonable sized cutter. So in real life you'll probably be lucky to be running 10m/min, particularly if the surface needs a good finish or high accuracy.

Together all these factors mean that you should be just fine with any modern machine, capable of this kind of work. If you are lucky enough to have a 100.000-200.000RPM spindle, my guess is that the controller will be happy chomping through the code - or you'll be driving it directly with equations or NURBS.

# Re: Relation 'intol outtol' and CNC code lines for freefrom machining

Siemens Legend
Would the lines per unit-time that a controller can read & process be much faster (smaller) than the time the machine would take to move? I would think, it's pretty hard to reach that threshold, unless you are running a very long tool path with very tiny steps (result of very small intol/outtol) and cutting in a very high feed.

# Re: Relation 'intol outtol' and CNC code lines for freefrom machining

Gears Esteemed Contributor

Older controls did have issues processing lots of little steps.

Older DNC systems as well, if you were "drip feeding" the data (depends on baud rate vs. feed rate)

But with newer machines/controls & lots of local memory (so you can copy the file locally, instead of drip feeding it) those problems should be much reduced (if not eliminated)

Ken Akerboom Sr CAx Systems Engr, Moog, Inc.
Production: NX10.0.3.5 MP16/TC11.2
I'd rather be e-steamed than e-diseaseled

# Re: Relation 'intol outtol' and CNC code lines for freefrom machining

Siemens Legend
Oh ya, those Pratt & Whitney having hydraulic pumps wrapped with diapers (but still leak). They can only read & digest one or two blocks at a time. And every block needs to have feed rate specified. We used to call that P format or something.