Slightly wrong size end result

[Dan B]

Can you change your "maximum distance, edge to surface" to 0.02 and on the units page change your absolute tolerance to 0.002?

Rerun your test and see what happens. I'm grasping at straws here, but I know my set-up doesn't have your issues, so it's worth a shot.

Dan

[matt3o]

I believe I started from 0.02 in the "edge to surface" and tried 0.05 later. Anyway I'll give it a shot, just to be sure. Absolute tolerance from 0.01 to to 0.002 is a big jump... let's see what happens.

Thanks!

[Mauri R]

Matt30,
I use Mach 3 with my CNC equipment and have no issue with accuracy.
I ran the simulation using 3.175mm end mills on both examples using the simulator and they both produced the same result this program always replicates what I get with the CNC machines.
My previous simulations were to demonstrate that the inner cut was within .01mm of each other (i.e.) it just nicked the edge.
In this example simulation, it shows that they are also very close on the outer cut.
I used a Square block with the dimension of 26.54 x 26.54 x 20 and a cutter of 3.175mm.
I also ran both again with the block size of 26.53 x 26.53 x 20 and they still look very similar in cuts.
can you provide the Rhino/madCam example so I can run it and compare the output.
Regards
Mauri.

MadCAM example header.
(BEGIN PREDATOR NC HEADER)
(MCH_FILE=4AXVMILL_MM.MCH)
(MTOOL T31 S1 D3.175 C0 A0 H51 SD3.175 SH1 HT1 HD34 HH20)
(SBOX X-13.27 Y-13.27 Z-20 L26.54 W26.54 H20)
(END PREDATOR NC HEADER)
G00 G49 G40 G17 G80 G50 G90 G64 G21
(FLAT_END_3.175)
T31 M06
M03 S16000
G01Z1.587
G00X11.677Y6.513
Z1.587
G01Z0.000 F300
Y11.675Z-0.908 F1500
X11.167Y11.677Z-0.998
X-11.677Y11.675
X-11.675Y-11.677
X11.677Y-11.675
Y3.046
Y11.675
etc.

MeshCAM example header.
(BEGIN PREDATOR NC HEADER)
(MCH_FILE=4AXVMILL_MM.MCH)
(MTOOL T31 S1 D3.175 C0 A0 H51 SD3.175 SH1 HT1 HD34 HH20)
(SBOX X-13.27 Y-13.27 Z-20 L26.54 W26.54 H20)
(END PREDATOR NC HEADER)
%
(FILENAME: cube-mach.nc)
(STOCK/BLOCK, 26.350, 26.350, 20.000, 13.175, 13.175, 20.000)
G21G64G17
G90
(TOOL/MILL,3.1750,0,17.0000,0.0)
T31 M06
M3 S16000
G0X0.000Y0.000Z2.540
(Parallel Rough)
(Roughing Level Depth: -0.999)
G0X9.792Y11.681
G1Z-0.999F300.0
G1Z-0.999F1500.0
X9.436Y11.681Z0.000
X9.080Z-0.999
X8.723Y11.681Z0.000
X8.367Z-0.999
X8.011Y11.681Z0.000
X7.655Z-0.999
X7.299Y11.681Z0.000
X6.943Z-0.999
X6.587Y11.681Z0.000
etc.

[Dan B]

Absolute tolerance should be 10x what you actually want to achieve. For us, ±0.02mm is typically what we need to achieve, so that's why we use an absolute tolerance of 0.002mm. It may be tighter than what you require, but it's worth a try to see what happens.

[matt3o]

I made a very stupid error in the stock setup today and thrown away one day of work. Tomorrow I'll try again and see if the new configuration solved my issue.

Absolute tolerance should be 10x what you actually want to achieve. For us, ±0.02mm is typically what we need to achieve, so that's why we use an absolute tolerance of 0.002mm. It may be tighter than what you require, but it's worth a try to see what happens.

very interesting. hopefully that is the problem.

@Mauri, thanks again for running it through the simulator. I start to believe that there's a combination of events that causes this issue. I'll make one last test tomorrow and then throw the towel :P

[Dan B]

Before you give up on madCAM, send me your file privately if you can. I promise it won't be seen by anyone else other than possibly Joakim if I can't solve it. I want to analyze your model and your paths and see if I can figure this out. It has to be something in your process, as the software is a proven performer.

cncdanb@gmail.com

Dan

[svenakela]

Did you try to run the program without G64? It will not make a difference in any simulator, you have to try it in the machine.

G64 is blending lines to keep the cutter speed up, to make that happen the controller is allowed to make shortcuts - is, corners will be radius.
It might be that you have to replace G64 with a G61 to make sure it will kick in.

[matt3o]

maybe I've got an idea about what is happening... Most of my mills have a bigger shaft than the actual end mill size. meshcam has automatic collision detection, madcam does not. Meaning that in some situations meshcam will keep the endmill farther away from the part than what madcam does. That doesn't explain why even pockets end up smaller than what they should, though.

Thank you Dan for your help, really appreciated. Tomorrow I'll make this last test with the updated settings and if it doesn't work I'll send the model to you, maybe I'm just doing something really stupid during the paths creation.

Did you try to run the program without G64? It will not make a difference in any simulator, you have to try it in the machine.

I will also try this. Thanks.

[Mauri R]

matt30,
Analysing the two output sets of numbers they are different so the cuts will be different.
Because MeshCAM does an unusual start to the cutting process it is difficult to see in the first side cut around the block but it is quite visible in the last three sides.
So without a copy of the model Dan or I cannot see if I can replicate the same result.
MeshCAM madCAM
X11.471Y10.762 Y11.675
X11.344Y10.998 X11.167Y11.677
X10.998Y11.344 X-11.677Y11.675
X10.525Y11.598 X-11.675Y-11.677
X10.158Y11.639 X11.677Y-11.675
Y3.046
Y11.675
X9.792Y11.68 X11.167Y11.677
X10.370Y11.544 X11.037Y11.480
X10.678Y11.436 X10.906Y11.283
X11.080Y11.167
X11.081Y11.164 X11.167Y11.080
X11.436Y10.678 X11.446Y10.660
X11.544Y10.370 X11.583Y10.152
X11.589Y10.015 X11.591Y9.645
Y-9.879 Y-9.645
X11.572Y-10.234 X11.583Y-10.152
X11.475Y-10.589 X11.446Y-10.660
X11.278Y-10.944 X11.167Y-11.080
X11.081Y-11.163 X11.080Y-11.167
X10.914Y-11.300 X10.660Y-11.446
X10.370Y-11.544 X10.152Y-11.583
X10.015Y-11.588 X9.645Y-11.591
X-9.879 X-9.645
X-10.234Y-11.571 X-10.152Y-11.583
X-10.589Y-11.474 X-10.660Y-11.446
X-10.914Y-11.300 X-11.080Y-11.167
X-11.277Y-10.944 X-11.167Y-11.080
X-11.474Y-10.589 X-11.446Y-10.660
X-11.571Y-10.234 X-11.583Y-10.152
X-11.588Y-9.879 X-11.591Y-9.645
Y10.015 Y9.645
X-11.544Y10.370 X-11.583Y10.152
X-11.413Y10.726 X-11.446Y10.660
X-11.163Y11.081 X-11.167Y11.080
X-10.944Y11.278 X-11.080Y11.167
X-10.678Y11.436 X-10.660Y11.446
X-10.234Y11.572 X-10.152Y11.583
X-9.879Y11.589 X-9.645Y11.591
X10.015 X9.645
X10.370Y11.544 X10.460Y11.579
X10.906Y11.283

Regards,
Mauri.

[matt3o]

Thank you Mauri, I can't post the model publicly but I will be sending it privately after today's last test.

[matt3o]

I finally got it working (almost ). Honestly I don't know what was the problem. I reset my mach3 and recalibrated the motors and I updated the options as suggested by Dan. I also lowered the tolerance on the smaller cutters.

The end result is impressive.



The base of this thingy came out 18.0mm straight. The circle on top is exactly 11.0mm. I'm really impressed, never got such definition.

Only problem is in the bottom (not pictured), there's a little 5.4mm stem inside that came out 5.1mm instead (again 0.3mm !). Considering that everything else is perfect I suspect the problem could be in the cutter tolerance. The stem is outlined with a 3mm end-mill that is the only one with a higher tolerance (so lower definition), I guess for such small pieces I need to set very low tolerance. Otherwise I really don't know what to think.

Dan/Mauri, how do you set the tolerance when you need very fine details?

Thanks eveybody for your help, really appreciated. Now I just have to bite the bullet and hand €795, I'd love remachining but that's a little out of the hobbyist comfort zone. I'll give a spin at other products, but madcam is at the top of my list.

[Dan B]

I've never had to go tighter than 0.008mm on my tolerance for the tool. I seem to recall going tighter when I first started using madCAM but the processing time grows when the tolerance is tight. Through experimentation, I found the 0.008mm tolerance was a good balance between processing time and acceptable results.

Just had a thought...Did you check your tool for run-out? If everything else turned out exact, maybe the issue is with a specific tool. You most likely checked the diameter and it was fine, but run-out will cause your finished piece to be undersize even if the diameter is spot on. I'm specifically referring to the type of run-out caused by how the tool is held in the machine as opposed to a problem in the tool itself (which would be less likely unless your tooling is low end).

[Mauri R]

Matt30,
We main do 3D fine engravings in Timber and Brass although we have machined items accurately in Aluminium, however I like to be very accurate as well.
When I have tight tolerances set in Rhino and madCAM on complex large 3D models it can take hours to calculate on a fast PC.
Also you have to know your machine Capability, Tolerances, Spindle run-out, tightness of Gibbs and Steppers vs Servo's being some.
In Mach 3 there are some settings that can affect tolerance and you need to be sure that you have set these properly. (If you use CV control then CV Distance Tolerance and Stop CV in Angle are also important in obtaining accuracy) as well if you are using Steppers correct motor settings is important.
Once you have all this knowledge then you can set Rhino/madCAM software to obtain these tolerances to ensure a good machined outcome.
I try to achieve tolerances in the .01mm range and set my setting accordingly.
Regards,
Mauri.

[svenakela]

I am not doing a blame game here, but these kind of threads appear every now and then. In the end, it's a setting somewhere in Mach.
I rarely use less tool tolerance less than 0.02 mm and if I do it's 0.01. That's about what the work piece will expand when I open a cold beer...

[matt3o]

thanks for your continued feedback.

my original post originated from the fact that with basically no config I was able to obtain more precise pieces with meshcam than I could with madcam. Which seemed absurd. After some time and your help I was able to get quite some remarkable results with madcam but still I have some issues. Meshcam probably is more forgiving and takes some liberties while madcam does exactly what you say it to do.

I work on very small pieces, so lowering the tolerance shouldn't be an issue. Unfortunately the most important piece of my model is the inside "stem" that must be 5.4mm with a very little margin for error. I do not have tools to measure the run-out but the collet is the same for all the cutters so it shouldn't be that bad. I'll double check my 3mm end mills, maybe it's a problem with one of them and I simply used one when I milled with meshcam and another with madcam.

@svenakela, you can safely play the blaming game, I'm sure it's my fault, I'm just trying to understand what I'm doing wrong. Like I said, saying that I'm a rookie is an understatement.

[Dan B]

All you need to check run-out is an indicator. Zero the indicator at the top of the flutes by sweeping the flute past the indicator tip by hand. Raise the tool in the Z, so that the indicator tip is at the bottom of the tool and sweep the flute past the indicator tip again. Is it still reading zero?

A universal indicator is better for this than a dial indicator but a dial indicator will work.

As for tolerancing, it depends what you are doing. We work to tolerances 10X that of the part we are gauging. For us, finishing to within 0.01mm is something we do regularly, but we do check in our temperature controlled QC lab. Maybe my suggested 0.008mm tolerance is tighter that most would need. I often forget that madCAM is used for a wide variety of applications, and most probably don't have results qualified in a lab.

Dan

[matt3o]

just for the sake of completeness and for future reference... I made some more tests and it seems that I really need 0.01 tolerance or better to get satisfactory results. Surely configuring madcam has been more complicated than other cam software, but I really like how it works. Thanks everybody for your help!