PDA

View Full Version : Taig/Mach3 issues with accuracy



diamondback21
04-03-2009, 02:23 PM
I bought a used taig cnc milling machine(MicroProto) from this site back in December of 08. Im now where I can do quite a bit of stuff with it. Problem is when I try to cut a circle thats .430" it comes out to .452" i cant seem to figure out the the problem is. I have the machine set up true as far as tram, backlash, etc. I am using Mach3. Axis XYZ all have .001" of backlash. I have compensated for it in Mach 3. All gibs and such are tight without any play or unwanted movement. I just dont understand why its doing this. Its really starting to get under my skin. I cant deal with that much difference. Does anyone know why this is happening. Im puzzled. Thanks for any help.

Jeff-Birt
04-03-2009, 04:25 PM
It sound like it might be a set up issue. I would first look at the steps per unit setting and then look at how you are doing cutter compensation.

escott76
04-03-2009, 04:33 PM
In the program run screen of Mach3 it will have a line which shows all the active G codes. Check to make sure you aren't for some reason in cutter comp mode. Not knowing a number of things about your setup or code it's difficult to diagnose, but also check things like how your IJ mode is set, and if you are using cutter comp make sure you have set the correct cutter diameter, are using the right offset, and are using the correct (41/42) comp code for the circle you are trying to cut.
Is it only during circles, or does this "cutting large" happen with any programmed path?

diamondback21
04-03-2009, 08:02 PM
yes, it cuts large no matter what. i have g-codes and m-codes in the program run screen. im using the cut circle program in mach 3. im using a 1/4" end mill with a diameter of .2470" and i put it in the program as such. my steps are set at 8000. motors are 30 vel. and 8 acc. for all axis. hope this helps.

escott76
04-03-2009, 09:18 PM
yes, it cuts large no matter what. i have g-codes and m-codes in the program run screen. im using the cut circle program in mach 3. im using a 1/4" end mill with a diameter of .2470" and i put it in the program as such. my steps are set at 8000. motors are 30 vel. and 8 acc. for all axis. hope this helps.

Consistent (error the same regardless of part size or cut) means that you have something off in your cutter comp settings. It can be a little confusing to get right. Pay attention to your cutter comp entry and exits. Give it space to get to where it needs to go to clear the area.

TOTALLYRC
04-03-2009, 10:07 PM
If you haven't done it already, use a dial indicator and see if a 1" move results in one inch of travel on all three axis. if not use the mach3 wizard for setting the steps per inch. You are off by .022 which is a large amount.

On my Taig, the steps per inch should be (according to the math) 16,000/inch as my drive is set to 1/8th step but my steps per inch needed to be adjusted slightly to some weird number like 16,023.54 to make it move exactly 1 inch.
Since you haven't mentioned it, I will assume that you are not using g41/42 to set cutter comp.

On my bridgeport, my 5 tpi screws should give me 20,000/inch, but they are actually metric which gives a real weird number when using inches, so the math is correct, but only if you know the actual numbers to input.
Once you have the dial indicator moving one inch when you try to move one inch, I would try cutting a square in some scrap material as you can hand code it really easilly. The move on to a circle.

The other thing to check, and it has caught a lot of people, is to use a second measuring device to verify your measurements. One guy here on the zone was going nuts with an odd table movement dimension and found out that his dial indicator had a cyclicle error and once he had a good indicator, he had everything perfect.

Mike

diamondback21
04-03-2009, 11:14 PM
Ok i used a different offset. dont think this matters . cut a rectangle pocket .7500"x2.2500" and it was dead on. i cut a circle that was supposed to be .5120" and it came out to .5265" i also went to general config and logic config. and unchecked the radius comp off box just to see what would happen. hope this helps. thanks

diamondback21
04-03-2009, 11:42 PM
i have the microproto 2000hd/le. i think the 2003 model. the manual says to use 8000 steps per. i changed it to 16000 and still comes up .001" short of 1". i changed the backlash to .002" still no difference. it came up.001" short. im about to pull whatever hair i have out.

ger21
04-03-2009, 11:46 PM
If you turn off backlash comp, what do you get?
Also, try at different feedrates (slower) and see if you get the same results.

escott, I'm pretty sure he's not using cutter comp.

diamondback21
04-04-2009, 01:56 AM
i fine tuned the steps per in the settings menu. and got it to .5175". i disabled backlash comp and slowed the feed down to 6ipm and got a .5195" circle. im not using g41/42. im using the circle cut wizard in mach3. even with my cad/cam programs dimensions. they're off just as much. maybe it just worn out.

TOTALLYRC
04-04-2009, 03:09 AM
i fine tuned the steps per in the settings menu. and got it to .5175". i disabled backlash comp and slowed the feed down to 6ipm and got a .5195" circle. im not using g41/42. im using the circle cut wizard in mach3. even with my cad/cam programs dimensions. they're off just as much. maybe it just worn out.

If the machine is worn out, your rectangle would have not come out dead on.

Keep playing with the steps per inch, untill it is correct. so if you have to go to 16,035 or something weird, as long as the movement is correct, it is ok.

If your circle is coming out round, but to a different dimension than what you are asking, and your squares are correct, then it sounds like it is an error in the gcode, and not the machine. If you had a worn machine and a ton of backlash, your circle would be flatted at the compass points and the rest of it would be close in size.

Post the code you are using to cut a circle so we can check it out plus the actual cutter diameter and the measured result.

Mike

Hirudin
04-04-2009, 03:47 AM
Regarding the possibility that the machine is worn out... My brand new Taig has been cutting parts a bit big too. I'm fairly sure all my gibs are properly adjusted and after adjusting the nuts I've been leaving backlash compensation turned off.

I don't know what cutter compensation is, and I doubt I'm using it.

Also, I set my steps per using a gauge block, so I think it's set very close to what it should be.

TOTALLYRC
04-04-2009, 04:15 AM
Regarding the possibility that the machine is worn out... My brand new Taig has been cutting parts a bit big too. I'm fairly sure all my gibs are properly adjusted and after adjusting the nuts I've been leaving backlash compensation turned off.

I don't know what cutter compensation is, and I doubt I'm using it.

Also, I set my steps per using a gauge block, so I think it's set very close to what it should be.

Using a gauge block and a good .0001 dia indicator, you should be dead on and very repeatable. cutter comp is set using the G41/g42 and turned off using the G40? command. if you are not sure what it is, good bet you are not using it.

Parts "a bit big" is very vague. If you are within a thou or 2 you start getting into the realm of cutter flex and machine flex. If you are talking less than tenths, the room temp and machine temp starts to come into play .

I always try to use a roughing pass and then a finish pass when I am going for close tolerances. You will cut the first part, measure it and then use the cutter comp to get closer to the proper size. This is where the art of being a machinist comes in. Even if the cam program gets it right and the machine is perfect, somtimes the cutter cutts differently than you would think based on its size.
:withstupiSometimes you measure the cutter wrong.:withstupi

:bat:Sometimes the wind is blowing the wrong way with the part you are cutting.:bat:

(chair)Sometimes the material is not what you think it is and it cuts differently.(chair)

Mike

Hirudin
04-04-2009, 05:54 AM
Heh... sorry for being vague. I couldn't remember any exact measurements so I thought it would be best not to say anything specific. If I remember right some measurements were off 7 to 15 thousandths. When I took the measurements I thought it seemed too large to be explained by the cutter being slightly smaller than I expected.

I've tweaked my machine here and there, I'll have to do a controlled test and come back with real numbers... :o

I've started doing the roughing/finishing passes too. I started doing it to try to get better surface finish, but I find it also gives me a little buffer room if I have to re-zero the machine at some point. I've decided to leave 10 thousandths when roughing. I figure that means it's less necessary to get down to the last thousandth if I ever have to zero the machine again. Then I try to do the finish pass all at once.

diamondback21
04-04-2009, 12:32 PM
heres the code for the circle and i also ran a another rectangle pocket 2.125"x1.25 and it came out 2.1305x 1.2535"F6 I fine tune the steps per to where they,re moving exactly 1" . im gonna do some more test. I dont think its consistent.
G00 Z0.25
G00 X0.12875 Y0
G00 Z0.5
G01 Z-0.007 F5
G02 X0.12875 Y0 I-0.1287 J0 F6
G01 Z-0.014 F5
G02 X0.12875 Y0 I-0.1287 J0 F6
G01 Z-0.021 F5
G02 X0.12875 Y0 I-0.1287 J0 F6
G01 Z-0.028 F5
G02 X0.12875 Y0 I-0.1287 J0 F6
G01 Z-0.035 F5
G02 X0.12875 Y0 I-0.1287 J0 F6
G01 Z-0.042 F5
G02 X0.12875 Y0 I-0.1287 J0 F6
G01 Z-0.049 F5
G02 X0.12875 Y0 I-0.1287 J0 F6
G01 Z-0.056 F5
G02 X0.12875 Y0 I-0.1287 J0 F6
G01 Z-0.063 F5
G02 X0.12875 Y0 I-0.1287 J0 F6
G01 Z-0.07 F5
G02 X0.12875 Y0 I-0.1287 J0 F6
G01 Z-0.077 F5
G02 X0.12875 Y0 I-0.1287 J0 F6
G01 Z-0.084 F5
G02 X0.12875 Y0 I-0.1287 J0 F6
G01 Z-0.0898 F5
G02 X0.12875 Y0 I-0.1287 J0 F6
G00 Z0.25
G00 X0.13275 Y0
G01 Z0.4062 F6
G01 Z-0.0938 F5
G03 X0.13275 Y0 I-0.1327 J0 F6
G00 Z0.25
G00 X0 Y0
M30

TOTALLYRC
04-04-2009, 02:34 PM
heres the code for the circle and i also ran a another rectangle pocket 2.125"x1.25 and it came out 2.1305x 1.2535"F6 I fine tune the steps per to where they,re moving exactly 1" . im gonna do some more test. I dont think its consistent.
G00 Z0.25
G00 X0.12875 Y0
G00 Z0.5
G01 Z-0.007 F5
G02 X0.12875 Y0 I-0.1287 J0 F6
G01 Z-0.014 F5
G02 X0.12875 Y0 I-0.1287 J0 F6
G01 Z-0.021 F5
G02 X0.12875 Y0 I-0.1287 J0 F6
G01 Z-0.028 F5
G02 X0.12875 Y0 I-0.1287 J0 F6
G01 Z-0.035 F5
G02 X0.12875 Y0 I-0.1287 J0 F6
G01 Z-0.042 F5
G02 X0.12875 Y0 I-0.1287 J0 F6
G01 Z-0.049 F5
G02 X0.12875 Y0 I-0.1287 J0 F6
G01 Z-0.056 F5
G02 X0.12875 Y0 I-0.1287 J0 F6
G01 Z-0.063 F5
G02 X0.12875 Y0 I-0.1287 J0 F6
G01 Z-0.07 F5
G02 X0.12875 Y0 I-0.1287 J0 F6
G01 Z-0.077 F5
G02 X0.12875 Y0 I-0.1287 J0 F6
G01 Z-0.084 F5
G02 X0.12875 Y0 I-0.1287 J0 F6
G01 Z-0.0898 F5
G02 X0.12875 Y0 I-0.1287 J0 F6
G00 Z0.25
G00 X0.13275 Y0
G01 Z0.4062 F6
G01 Z-0.0938 F5
G03 X0.13275 Y0 I-0.1327 J0 F6
G00 Z0.25
G00 X0 Y0
M30

Notice on the bold line that your I number is different from all of the previous lines. This will cause the bottom of the part to be bigger and it may cause the discrepency that you are getting, especially if you can't see the step.

I wonder what you are using to measure these parts. If it is a set of digital calipers, verify that they are repeatable and are reading what they are supposed to. I notice that you pocket is measured to .0005 and unless you are real good with an inside micrometer, you can't measure them that close.

Mike

diamondback21
04-04-2009, 05:50 PM
i checked and rechecked the steps per unit with 3 different dial indicators. all read the same. im still getting a circle that roughly .01"larger than what i want. i also measured the circle with 3 different dial calipers. I even went out a bought a new one just to be sure the other 2 were not off. all give the same numbers. (chair)

diamondback21
04-04-2009, 05:57 PM
Notice on the bold line that your I number is different from all of the previous lines. This will cause the bottom of the part to be bigger and it may cause the discrepency that you are getting, especially if you can't see the step.

I wonder what you are using to measure these parts. If it is a set of digital calipers, verify that they are repeatable and are reading what they are supposed to. I notice that you pocket is measured to .0005 and unless you are real good with an inside micrometer, you can't measure them that close.

Mike
its not just with this circle cut that the circle is too big, its with anything i cut. even parts that i have in my cad/cam program. the G03 line is the finish cut i have been using. this particular circle cut wizard in mach 3 is just to check and see if im getting close .

TOTALLYRC
04-05-2009, 01:30 AM
I would love to help out more, but you seem to have done everything that I would have done.

I will keep watching to see what other people have to contribute.

What is driving me crazy, is that if your step per in on the x and y are correct, and you only have a thou or two of backlash, you circles should be way closer than they are.

Mike

fretsman
04-05-2009, 09:02 AM
Ok, just had a thought, what are your "Scale" DRO's reading on the "Program Run" page?

Dave

TOTALLYRC
04-05-2009, 10:44 AM
Ok, just had a thought, what are your "Scale" DRO's reading on the "Program Run" page?

Dave

Hey Dave.

That could be it. They should be reading 1.0000. anything else will scale the part to a larger or smaller size.

Mike

diamondback21
04-05-2009, 11:24 AM
the dro is reading 1.0000" I really appreciate the help. I just wanted to make sure i have covered everything. To make sure I wasnt missing something. When i enter the backlash amount in the backlash tab. should it be entered as
ex.(-.0012) or just (.0012)?

Thanks

fretsman
04-05-2009, 11:49 AM
Damn! I was hoping that was it...... lol!

As for backlash comp, no, the manual mentions nothing about negative numbers.

Dave

diamondback21
04-06-2009, 08:16 PM
Well, I got it down to .007" from changing a few things. I was hoping for a little better tolerance. I dont know what else to do. Anybody know of any settings or configurations that I may have wrong?

diamondback21
04-06-2009, 10:54 PM
i just ran another circle cut with the Mach3 wizard. I said what the hell, lets enter the endmill dia. .007" bigger than Im actually reading on the dial caliper. The circle diameter was dead on!!! Im puzzled??????

BobWarfield
04-07-2009, 01:03 AM
diamondback, I am going through some similar pain with my newly CNC'd mill.

What things have you changed that improved the situation so far?

I got a big improvement from calibrating steps/inch properly. But I got an even bigger improvement in accuracy when I discovered that my endmill was not the diameter it was advertised as. In fact, it was off by a surprising amount!

I had a 3/16", which should have been 0.1875". I tried several different measurements on it including calipers and micrometer. In the end, I got the best result by taking a little piece of aluminum, measuring its length, slicing it in half with the endmill, measuring the lengths of the two pieces and realizing the difference was the endmill's diameter.

Be sure to run a similar check on your endmill!

I asked a number of machinist buddies how often they were seeing endmill's that were off and their answers varied. It boiled down to expensive endmills being very close (tenths) and other endmills being highly variable.

I still have some more tuning and testing to do, but I'm now within about a thou on most dimensions. I'm confident I can do quite a bit better when I get done with the other tuning work.

Cheers,

BW

diamondback21
04-07-2009, 08:54 PM
Hi Bob, Thanks for the tip. I used a 1/4" endmill that was .2820 on the calipers and then a straight run in aluminum and measured the cut width. Roughly.2900".
Then a circle test at 18ipm.Very quiet and very smooth. The circle was really nice and came out dead on. Some things I changed were wheel speed setting in config-general config and set the wheel speed setting to .00001. The default was .25 It runs through the circle faster at .00001 without stalling so to speak. If this makes sense. My motor setting are velocity-25 accel-10 and step pulse and dir pulse are both set to 5. I can run it great at 30 on the velocity. No stalls just very smooth. The difference in the caliper measurment and the cut width measurment seems to be alot. .009" U think I may have a bent spindle? Also any body know how to adjust the tram in the Y axis. Mine is waaaayyy off. .03" Do I have to shim it or is there something I need to adjust?

BobWarfield
04-07-2009, 09:40 PM
diamondback, RE the difference in caliper versus cut, there are a lot of things that can contribute to that.

Very likely you are getting some deflection on your machine from somewhere. You can try to minimize that by cutting the slot for the circle and then doing a finish pass where the endmill doesn't have to work very hard.

There is likely some runout as well. I hesitate to say that your spindle is bent--I would think if that were the case you'd see some vibration. But there are a lot of sources of runout. You'll have to do a fair bit of work to track it it all down if you want to eliminate it.

For example, you may be experiencing runout from:

- The toolholder. Are you using a collet chuck? R8 collet? Endmill holder? Any of these may be a source of runout. This is a very likely source of runout. You can look for better toolholders.

- The spindle itself. Indicate the inside taper of the spindle. Fix your indicator to the table, reach the point up inside, and gently rotate the spindle by hand to see how much the max deflection is over a full rotation.

Spindle runout can be a lot of things. For best precision, they should have cut the taper (ground it actually, but many are milled on cheap machines) while the spindle rotated in its own bearings, rather than cutting it and sticking it into a set of bearings later. This ensures the bearings and taper are concentric. Again, most cheap machines will not take this step.

Also, beware calipers for really accurate measurement. It's hard to use them accurately, especially to measure something like an endmill. Get a micrometer, it's worth it!

Isn't the amazing thing not that you have 9 thou discrepency there, but that you have 40 thou discrepency in the endmill's advertised size? That's the part that surprised me.

Best of luck with continued tuning. You're getting there!

Myself, I just got a package from Digikey--capacitors to fix the dread HEDS encoder noise problem Mariss F discovered. I don't know that I have the problem, but I have HEDS encoders and fairly long cables and this is cheap insurance. We'll see if it changes my accuracy at all. Encoder noise is not something a servo system will "fix" on its own, so could be.

Cheers,

BW

diamondback21
04-08-2009, 04:10 PM
On the Y axis when I jog the table from one end to the other, Theres about .03" difference. Is there a way to adjust this to make it run true?

diamondback21
04-08-2009, 06:02 PM
On the Y axis when I jog the table from one end to the other, Theres about .03" difference. Is there a way to adjust this to make it run true?

Never mind dont ask. Its only .001. Other than that, Its running great, cutting true. :cheers:I did have to set the velocity a little lower. It skipped a few steps when I ran a rectangle pocket. I lowered it to 2. It ran great between 5 and 7, but also runs great at 2. I will leave it where its at for now. Just to be sure. no more skipped steps. All is good now!!! I will continue to fine tune . Thanks to all that helped me thru this time of crisis. lol Hope this thread helped someone else out as well.