Thread: Hole interpolation accuracy with endmill

Originally Posted by Hardplates

It's been a while but I seem to remember being able to select the edge of the solid with contour which is not what you want. You want to hide the solid and make the sketch itself visible and select that. Maybe it's changed since I last used it since the bastards were making changes every week when I used it.

In many situations CAM packages interpret solid geometry selections as splines (depending on a host of issues including the originating CAD package kernel, any sort of hole edge distribution etc). Spline data is posted as a host of small line segments and will be controlled by chordal deviation tolerance, smoothing, and G187 type corner rounding in the control. By drawing non-projected lines and arcs, you can force the CAM system to use traditional code (G01, G02, and G03).

I suppose a person could make the case that the control then takes those G02s and G03s and applies a similar micro-segmenting algorithm; however, in most cases those are far less noticeable in surface finish and processing speed at the machine.

Point being, avoiding spline geometry in CAM pays dividends, especially running Haas type machines that have minimal look ahead. My understanding is the Japanese machine do far better digesting spline based CAM.


Sent from my iPhone using Tapatalk

CNC interpolated holes will never be "round" like a boring bar but who has a $50,000 gauge to check this?
For so many fits they are close enough and so easy to adjust to make any size even if only four point contact.
Becomes what is a "good" circle and then what is a good hole.
If making holes in a engine block you may get really fussy. If making a press fit dowel hole not so much.
Bob

Originally Posted by mhajicek

No contest indeed. I sometimes get a print and model at 5pm, and put the part on the engineer's desk by morning. I can throw an endmill in and get it done; I don't have a full set of boring bars for all length and diameter ranges. 99% of the time the hole will be a locating bore or a press fit for a pin, so if the gauge pins say it's good, it's good.

Not to mention the huge cost of a single boring head.

Originally Posted by G00 Proto

In many situations CAM packages interpret solid geometry selections as splines (depending on a host of issues including the originating CAD package kernel, any sort of hole edge distribution etc). Spline data is posted as a host of small line segments and will be controlled by chordal deviation tolerance, smoothing, and G187 type corner rounding in the control. By drawing non-projected lines and arcs, you can force the CAM system to use traditional code (G01, G02, and G03).

I suppose a person could make the case that the control then takes those G02s and G03s and applies a similar micro-segmenting algorithm; however, in most cases those are far less noticeable in surface finish and processing speed at the machine.

Point being, avoiding spline geometry in CAM pays dividends, especially running Haas type machines that have minimal look ahead. My understanding is the Japanese machine do far better digesting spline based CAM.


Sent from my iPhone using Tapatalk

That's pretty much what I was trying to get at. I believe most solids and surfaces are NURBS where sketch's are actual straight lines and arcs

Originally Posted by CORONA VIRUS

Not to mention the huge cost of a single boring head.

Good ones anyway. I have a couple cheapies I use once in a while.

0.0004 variation in hole size would likely mean the machine is cutting as good as it was ever stated to, your cutter is not deviating more than 0.0002" from the commanded position (per side). Assuming they go by the somewhat standard 0.0004" accuracy 0.0002" repeatability claims for machine that size/type.

If you feel you should be getting better results, there is one trick you can try. After interpolating one of your holes, have the program jog the machine around a good percent of the tables travel instead of just going to the next closest hole. On box way machines there is a tendency to "squeeze" out some of the way oil when you do a bunch of moves in one little area (i.e interpolation), increasing sticktion and perhaps causing some inconsistencies. Jogging the machine some distance between holes might redeposit a nice even film of way oil, possibly giving better results.

One trick to eek out a little more accuracy would be to alternate climb and conventional passes; that'll cover up axis reversal marks a bit.

I wanted to update everyone. It turns out that the people we bought the machine from were overcompensating the backlash. After setting the backlash comp to zero on all axes, I get about 50 millionths backlash in all axes. lol

Originally Posted by cgrim3

I wanted to update everyone. It turns out that the people we bought the machine from were overcompensating the backlash. After setting the backlash comp to zero on all axes, I get about 50 millionths backlash in all axes. lol

When buying a used machine many people will check backlash with an indicator, but few check the control backlash values against the factory parameters

Backlash comp done with a indicator and simple step moves back and forth is almost always wrong and way overdone.
Bob

Most indicators have some hysteresis, which will appear to be backlash.

Even with LVDTS there is static and dynamic motion and how servo loop work.
End position is not running at 1500 IPM.
This a rabbit hole with no end. Control loop people love this math. Arc is analog yet the control is digital and time sliced.
What goes on between each time slice that the control sees, what are the time contrasts both electrical and mechanically.... Its a wonder these things work at all.
Bob

I did not write a program to check backlash. I just checked it with a 50 millionths indicator with the jog handle. I know the best way to do it is to write a program but I haven't had time to do that yet. I will do that this weekend.

I just changed the normal backlash comp. There is a rapid backlash comp too. Should I change this as well?

Originally Posted by cgrim3

Coronavirus, I'm not entirely sure how to do that in fusion. I don't think fusion gives you that level of control but I might be wrong

I think you'd have to change the post to get that result in the code. Once upon a time controls required that you output quadrants, so it can be done. I don't think it would be as simple in Fusion as drawing 4 arcs. Might be easier to just hand code it if it's all circles.
FWIW the HSM Post forum could probably tell you how to do it overnight, even how to toggle it on and off.
HSM Post Processor Forum - Autodesk Community

To address the concern about whether you should select geometry or a skecth in Fusion 360 for creating your toolpath, I posted this question over on the fusion 360 manufacturing forum. We will see if any of the autodesk people respond.

Chris

Originally Posted by cgrim3

To address the concern about whether you should select geometry or a skecth in Fusion 360 for creating your toolpath, I posted this question over on the fusion 360 manufacturing forum. We will see if any of the autodesk people respond.

Chris

Try selecting geometry and posting code, then select a sketch and post the code and compare.

I just tried opening fusion to give it a try and it won't run unless I update it by downloading the latest version. So there is a better chance of hell freezing over than me trying it.

Give me a sec I'm going to try it. Do you guys use ijk's or R's?

I created two different programs for interpolating a 1.002" hole with a .5" endmill. One program I just selected the geometry of the hole and on the other program, I selected a sketch I created. The programs are identical. I am not saying they will always be identical though. All I did was just a quick and dirty experiment.

Does everyone here use i,j,k's or R's? I was always told to use i,j,k's because they are more accurate. What do you all think?

Originally Posted by cgrim3

I created two different programs for interpolating a 1.002" hole with a .5" endmill. One program I just selected the geometry of the hole and on the other program, I selected a sketch I created. The programs are identical. I am not saying they will always be identical though. All I did was just a quick and dirty experiment.

If the geometry selection was outputting 1 arc then the sketch selection will do the same as there is no way the code can get any more simple. Where selecting sketches should help is when the geometry selection outputs linear moves or tons of small arcs.

As far as arcs I run IJK. I don't know if they are more "accurate" but I remember hearing about bores not matching up well if your fourth decimal place was an odd number or something along those lines. Also I seem to remember R not being able to make a complete helix like IJK can. Anyway R has some limitation where IJKs only drawback is it's slightly more "complicated" to fingerCAM