Machsupport Forum

Mach Discussion => General Mach Discussion => Topic started by: s1000rr on July 25, 2012, 10:34:34 AM

Title: Cut parts are wrong size, CNC knee mill problem
Post by: s1000rr on July 25, 2012, 10:34:34 AM
Hi Guys,

I'm having a similar problem to the user in this thread: http://www.machsupport.com/forum/index.php/topic,21962.10.html

My setup:

Acer 5hp knee mill
Brushed servos
Granite Devices Servo Drives and interface card

This is my second cnc conversion but my first servo setup. I have brand new ballscrews in the machine, Hiwin ground screws with preloaded nuts.

I've set my travels with a mitutoyo digital dial indicator with accuracy of 0.001mm. My travels are accurate to within 0.002mm and it doesn't matter if it's 1mm or 100mm of travel. I have around 0.028-0.032mm of backlash on both axis that is 100% consistent.

The problem that I have is that my parts after being programmed in Solidcam were cutting outside diameters perfectly, but inside diameters were always 0.2mm too small. It didn't matter if it was a hollow circle, square, rectagle etc.. always 0.2mm. I adjusted feeds to super fast and super slow and always the same result. I rechecked the travels with the set steps function and it was always the same as mentioned above. I also tried cutting parts that were 2 inches thick, in 5mm step downs to see if the machine was missing steps as there woudl be ridge marks but it always cut perfectly. It doesn't make a difference if I cut 5mm deep, 12mm deep, 20mm deep, at 100mm a minute or 700mm a minute, the results are always the same. The bit has always been a new 3 flute, 0.5" diameter (12.7mm) carbide that just eats aluminum like butter.

Last night my dad suggested that I use the onboard wizards to cut a circle as I've used them on my smaller mill and it always generates code that cuts to size. The same problem occured, when I cut a circle or a circular pocket the diameter is always 0.2mm to small. So this has eliminated the cad/postprocessor and it has something to do with Mach3 but for the life of me I have no idea what could be wrong. There is no play in the table, no play in the angular bearings that support the ballscrews, the ballscrews are mint and 100% repeatable with 0.03mm of backlash, the servo drives are set to stop the machine if there is more than 30 encoder errors from target to destination (4000 encoder inputs per revolution, that's around 0.75% error) and based on my observation it never exceeds 15 errors.

Any ideas? I'm thinking of going back to the same version of Mach3 that my benchtop mill has but I don't know if I will be able to find it as it was installed 7 years ago.

Cheers,
Sebastian
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: Hood on July 25, 2012, 10:49:02 AM
I presume you are using the parallel port and if so then I would also assume you are using electronic gearing in the servo drives? If you are try with it off and see if it make a difference.
Is there any play in the spindle bearings or quill that could be deflecting the tool?
Hood
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: Overloaded on July 25, 2012, 10:59:58 AM
Hi Sebastian,
  Have you compared Climb to Conv. milling the same file ?
Could be a spindle issue ?

Russ
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: s1000rr on July 25, 2012, 11:05:53 AM
Parallel port yes. Electronic gearing: I don't think so but I'm not familiar with the question. I have a belt setup from the servos to the screws, and the bodies are heavy duty cast pieces that do not flex at all even under the heaviest of cuts (checked with my digital dial indicator). The entire head was rebuilt before the new screws were put into place with top of the line NSK bearings, no play there. If there was play I wouldn't be getting a near mirror finish on the edges. That's the strange thing that no matter the size of the part, the internal diamter is always 0.2mm to small.

Climb/conventional doesn't make a difference. Surface is near mirror finish so there is no chatter.

Sebastian
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: s1000rr on July 25, 2012, 11:10:29 AM
I've also tried Fanuc, Fanuc 5A, Mach3 post processor files and no difference. I've eliminated the cam side as the problem because the internal wizards in Mach3 reproduce the same problem, internal diamter circles are 0.2mm to small. But when setting the travels with the step config function, the table moves exactly how much I asked. This is the part that has me stumped because I'd understand if it was losing steps, or there would be ridges in the finish but nothing of that sort.

Sebastian
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: Overloaded on July 25, 2012, 11:32:32 AM
.... and of course you have verified that the code produced is EXACTLY as you are expecting for the given geometry and tool dimensions ?
sorry if this is too obvious, but I did not see it mentioned.  :)
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: BR549 on July 25, 2012, 11:41:44 AM
Are your cuts WITH tool radius comp or without?  Is the difference in cut symetrical around the part?

(;-) TP

Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: s1000rr on July 25, 2012, 11:48:43 AM
Yes, that is where the idea of eliminating Solidcam/Postprocessor and using the onboard cam wizards in Mach3 was mentioned. My dad suggested this to pinpoint where the problem was, Mach3 or Solidcam. Using the onboard cut circle or circular pocket wizard, I entered a circle diameter (tried several sizes progressively getting bigger) and 12.7 for the tool diameter and each time it was 0.2mm too small all around the circle.

Now I know that it seems that the grind on the bit is smaller than the 0.5" diameter of the shaft, but I've verified with my distributor that they are in fact 0.5" cut diameter with a tolerance of 0 -> -0.05mm of diameter just like the part number listed.

With the Mach3 circular pocket cut, I have no idea. Is there a tool comp setting in Mach3? I've never used this feature in the past.

Sebastian
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: Hood on July 25, 2012, 12:37:51 PM
I was just thinking if you have 4000line encoders and are using the parallel port then you would really need to have some electronic earing in the drives or your Velocity would be rather low.
Or were you meaning your steps per unit were set to 4000?
Hood
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: s1000rr on July 25, 2012, 01:21:47 PM
I don't understand what you mean by electronic earing? The drives have a gui interface that allows you to set it up based on your machine, you enter the type of servo, encoder count per rev, max current, voltage being entered into the drives min/max, you tune the PID and it shows you a digital oscilloscope, etc... The encoders go direct into the drives, how would using a parallel port affect the way they run?

 I also don't have them setup to run very fast, about 900mm a min max but I cut usually 12mm down and 10mm step over at 800mm/min so that is more than fast enough for me.

Sebastian
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: s1000rr on July 25, 2012, 01:23:24 PM
Also don't know if I mentioned but this problem isn't related to speed. If I turn the speed down to 100mm/min I get the exact same cuts as running 900mm/min. My acceleration is quite low also, 10mm/s/s.

Sebastian
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: Hood on July 25, 2012, 01:40:07 PM
Sorry earing should be gearing ;D
Sounds like you may not be using it but I will give a wee explanation anyway ;)
Ok when using servos with highish resolution encoders you will be limited to the max velocity you can get when using the parallel port. This is because the max pulserate of Mach is 100KHz but for most 60KHz is a likely max as it all depends on your particular computer hardware.
Ok so steps per unit.... say you have  4000 line encoders that is 16,000 pulses per rev as far as Mach is concerned. Assuming no mechanical gearing between the motor and screw and the screw being 5mm pitch your steps per unit would be 16,000/5 = 3200 steps per mm. Now if you had the kernel in Mach set to 25KHz that would mean the max Velocity you could achieve would be 25,000/3,200 x 60 = 468mm/min
 So say you find you can reliably pulse at 60KHz your max rapid would be 60,000/3,200 x 60 = 1,125mm/min
Now for most that is not a very fast rapid but that will depend on the machine for example 8 to 10m/min is sort of normal for a knee mill or lathe running servos. So as you can see that is not possible when using the parallel port, there are two things you can do.
1. Use electronic gearing if your servo drives support it, what that means is you tell your servo drive that every time it sees a pulse from Mach it treats it as say 5 or 6 or 10 etc. That way you can reduce your steps per unit in Mach by dividing by the electronic gearing ratio So say previously you were maxed out at 1,125mm/min as in the above example, if you had 5:1 electronic gearing you would now manage 5,625mm/min

2. The other option is to use an external pulsing device such as the smoothstepper, it can pulse up to 4MHz so you are unlikely to hit a velocity limit.

Now lastly, reason I asked about the electronic gearing was,  some of the lower end drives do not do it very well and can add a few or loose a few steps every now and then.

Hood
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: s1000rr on July 25, 2012, 02:36:53 PM
Ahh makes sense, I didn't know that such a thing even existed.

Can someone tell me more about tool compensation and where it's located? I've never used this nor set it up but I just want to make sure that it isn't set to something.

Sebastian
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: Hood on July 25, 2012, 06:32:46 PM
Your tool comp would be with a G41 or G42 in your code.
 I dont use the wizards much bit I dont think they use comp at all so it is unlikely to be your problem.
Hood
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: BR549 on July 25, 2012, 10:31:29 PM
Can you post the G code for one of your test circles. Earlier you said it cuts perfect on outside cuts but OFF on inside cuts is that still true??

What version of Mach3 are you running?

(;-) TP

Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: s1000rr on July 26, 2012, 10:21:58 AM
A little update. My dad said to cut a circle with the Mach3 wizard with the quill fully extended (around 6 inches) and barely extended, both times the circles had perfect finish and were 0.2mm too small. Following this I uninstalled Mach3 the latest most stable version (3.042?) and installed 1.84 which is the version that I have on my benchtop mill. I setup the travels again with my dial indicator and this time the circles were around 7.2mm too big. I triple checked the wizards settings, bit was 12.7mm but no luck every circle was a disaster. I then uninstalled and installed the latest development version. Reset the steps etc... Now the circle wizard was cutting within 0.08mm too small which I thought was great because the tool when brand new could be -0.05mm and it's cut a lot of aluminum so you could remove a couple more hundreths of a mm. I then proceeded to cut a test piece from solidcam and complete disaster, it cut the outside 0.2mm too big and the inside 0.2mm too small.

Everytime that I set the steps, I didn't copy the previous value I instead got the dial indicator out and set it with the configuration step option. Each version had a slightly different value, but between the most stable and dev version this difference was very small, while it was larger going back to the 1.84 version. I'll post gcode tonight, don't have it with me.

I'm running out of ideas.....

Sebastian
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: Hood on July 26, 2012, 10:35:34 AM
You have accurate balscrews, you know the count of your encoders and you I would imagine know the gearing between motors and screws if you have any. That is all you need to calculate the steps per unit. If you tell me the numbers I will calc it for you. Calculating is the most accurate way if your hardware is accurate.
Steps per unit do not change from version to version of Mach so there is something wrong if you are needing different values each time.

Also what kernel frequency do you have set?
Hood
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: s1000rr on July 26, 2012, 11:01:08 AM
Let me clarify, when going from the most stable -> the latest dev (3.0 something) the value changed by 0.1-0.3 something very small. When going from 3.0something to 1.84 it changed by around 10.

I'm sorry but I don't know that the ratio on the pulleys is as I purchased this mill with a damaged Anilam controller so the servos already the housings and belt conversion done, I just put in new ballscrews. Isn't that the point of the set steps funtion to make this calculation for you? It's not like I'm using an analogue dial indicator or a cheap brand with no reputation, it's digital and very accurate so that intrigues me as well as to why the values change. When I set the steps, I rerun the table to different distances using the step set function (but I don't type in the actual range travelled, just press esc to not change the set steps) ranging from 1-12mm and they are always withing 0.002mm.

It's the standard 25000, as I haven't changed it.

Sebastian
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: deejayspinz on July 26, 2012, 11:02:01 AM
I recently had this problem and figured out the cause.  First - alert - I'm a noob... but I know that this caused my issue.   I was having issues with my part cutting fine, but then a second part of the g-code causing the finishing stage of my part to cut approx 1" to the right of where it should be (mill ended up going out into the stock where it shouldn't).  I was recommended to try to slow down the feedrates etc..  What I did was play with the Motor Tuning section of Mach.  However, I did it blindly and it caused my issue.  My unit is setup for 4000 steps per inch (157.48/mm).  I left this value, but cut the other two (velocity & accell) in half.  This caused my part to be cut at approx half the size it should have been.  When I changed it back, it worked fine.  Not sure if this is the same issue you have, but worth checking to ensure you have your Motor Tuning setup correctly.

(http://www.piclist.com/images/member/RB-ezy-Q33/MACH3MotorTuning.jpg)
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: Hood on July 26, 2012, 11:17:29 AM
What are the steps per unit you have?
What line count are your encoders, you mentioned 4000 but not sure if that is the line count or the quadrature output?
What pitch are the ballscrews? I assume they will either be 5mm itch or 0.2inch pitch but will need to know.
With the above info I can calculate out as I will know roughly your gear ratio from your steps per unit and it is most likely that te gear ratio will be a round number. You could of course count the teeth on each piulley and get the ratio that way but if you let me know the above it should be straightforward. Measuring distance is ok but it will only be as good as your measuring . Even having  good measuring  gear will not be as accurate as calculating when you have good screws etc

Hood
Hood
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: s1000rr on July 26, 2012, 11:30:22 AM
1000 line encoders
5TPI ballscrews, 0.2"
The number is somewhere around 1179-1184

The problem is that it cuts the inside too small now and the outside too big. The only way to fix it is to reduce the cutter diameter by 0.2mm in the solidcam. Because if I decrease the steps per mm, then the outside will be to size the inside will be even smaller. If I increase the steps per mm, then the inside will be fine but the outside will be too large. If the outside was too big and the inside was too big, than that would indicate that the steps per mm was off. It's hard to explain, but do you sort of understand what I was trying to say?

Sebastian
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: s1000rr on July 26, 2012, 11:32:46 AM
One more thing, should I turn off "Enchanced Pulsing" or increase/reduce the step & dir time in the motor tuning window?

Sebastian
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: Hood on July 26, 2012, 11:47:17 AM
You could try with enhanced pulsing off but I would think it would be worse as 99.999% of people need it.
You could try increasing the pulse widths, try 10 and see or even enable sherline mode and see.
With your numbers I would say you have 1.5:1 gearing and that your steps per unit should be set to 1181.1023622

Hood
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: Overloaded on July 26, 2012, 12:01:20 PM
An interesting test.
 
Code and mill a circular slot like this sample.
If finished cut slot width is same as cutter dia., and the OD (boss) is correct, then how could the ID (bore) be too large ?  ? ?
...and vise-versa.
Here you are milling an OD and ID at the same time.
this will help to verify your measuring techniques as well as what the cutter is actually doing dimensionally.
Might lead to a clue.
Russ
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: s1000rr on July 26, 2012, 12:11:51 PM
My solidcam code test has been a horseshoe type shape as shown below. This allows me to pocket, lift z, lower z, and finish in one pass.

My plain circles have been generated by the mach3 cut circle wizard.

Sebastian
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: s1000rr on July 26, 2012, 12:15:12 PM
The horseshoe is the solid material left, revised pic.

Sebastian
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: s1000rr on July 26, 2012, 12:30:54 PM
Okay this is my idea of a game plan for tonight:

Brand new 3 flute 0.5" carbide ZRN coated bit (should be delivered today, says enroute)

Cut a 30mm circle with the following code that was generated by the Mach3 wizard:

F400
G00 Z10
G00 X8.55 Y0
G00 Z1
G01 Z-0.5 F50
G02 X8.55 Y0 I-8.55 J0 F400
G01 Z-1 F50
G02 X8.55 Y0 I-8.55 J0 F400
G01 Z-1.5 F50
G02 X8.55 Y0 I-8.55 J0 F400
G01 Z-2 F50
G02 X8.55 Y0 I-8.55 J0 F400
G01 Z-2.5 F50
G02 X8.55 Y0 I-8.55 J0 F400
G01 Z-3 F50
G02 X8.55 Y0 I-8.55 J0 F400
G01 Z-3.5 F50
G02 X8.55 Y0 I-8.55 J0 F400
G01 Z-4 F50
G02 X8.55 Y0 I-8.55 J0 F400
G01 Z-4.5 F50
G02 X8.55 Y0 I-8.55 J0 F400
G01 Z-4.9 F50
G02 X8.55 Y0 I-8.55 J0 F400
G00 Z10
G00 X8.65 Y0
G01 Z-4 F400
G01 Z-5 F50
G03 X8.65 Y0 I-8.65 J0 F400
G00 Z10
G00 X0 Y0
M30

Attached a pic below of the screenshot. Should I adjust my steps manually until this circle is exactly 30mm?

Then cut a 30mm profile circles with Solidcam gcode. If same size, then cut teh horseshoe?

Sebastian
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: Hood on July 26, 2012, 01:23:51 PM
Have you adjusted the steps per unit to what I mentioned?
Hood
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: s1000rr on July 26, 2012, 01:26:28 PM
No I'm currently at work, will set it to that first then cut the circle with the posted g-code and see the result.

Can you verify that the gcode is fine?

If it's too small/big, should I manually adjust the steps? For example too big -> reduce steps, to small -> increase steps

Sebastian
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: Hood on July 26, 2012, 01:33:47 PM
Code looks ok.
You have accurate ballscrews so if you have to adjust the steps from that calculated then you have something wrong and adjusting them by tweaking is not going to help in my opinion.
How are you measuring the ID and OD?
Hood
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: s1000rr on July 26, 2012, 01:44:07 PM
Yes I agree with you on the tweaking, that's just masking the problem and probably wouldn't work.

Sebastian
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: Hood on July 26, 2012, 01:57:20 PM
Not that it matters but just a bit curious where you are as you seem to be setting in metric, code is metric but your cutter is imperial.

Hood
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: s1000rr on July 26, 2012, 02:01:23 PM
Canada eh! I grew up with the metric system, but all of the cutters are imperial and are generally produced in the states. Metric ones are possible but then it's hard to find metric collets etc... Just easier, cheaper and more selection in imperial cutters over here. Some machinists here work in imperial for travels, cuts etc... but that just doesn't make any sense to me.

Sebastian
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: Hood on July 26, 2012, 02:18:24 PM
Ok makes sense now. We can get metric or imperial cutters here for the same costs but as I work in metric its normally metric cutters I use just makes it easier on my head ;D
Hood
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: BR549 on July 26, 2012, 04:16:41 PM
HERE is "simple" Code for an inside circle AND an outside circle. It is setup for a 4"center line .

Not saying it is BUT there may be a problem within MACH3s conversion to metric Gcode on the G2/G3.

Art always said IF you are going to normally CUT metric then set the machine to metric as well.

IF that cuts correctly both ways then we will try a metric Gcode via Imperial machine.




(Filename: Circle_4x4)
( Plasma Shape WIZARD )
(Date Created: 07/26/12)
(Time Created: 3:54:49 PM)
G20 G17 G40 G54 G80 G90
G0 Z0.5
G0X0Y0
G0 Y2
M3
G4 P3
G1 X0 F20
G0 Z0.0
G3 X0 I2 Z-.050
G3 X0 I2
G0 Z0.5
M5
M30


(Filename: Circle_4x4)
( Plasma Shape WIZARD )
(Date Created: 07/26/12)
(Time Created: 3:54:49 PM)
G20 G17 G40 G54 G80 G90
G0 Z0.5
G0X0Y0
G0 Y2
M3
G4 P3
G1 X0 F20
G0 Z0.0
G2 X0 I2 Z-.050
G2 X0 I2
G0 Z0.5
M5
M30
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: Hood on July 26, 2012, 05:04:16 PM
Terry his machine is set to metric and code is metric, it was just he was buying imperial cutters and I was curious why.
Hood
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: RICH on July 26, 2012, 05:45:07 PM
Hmm,
The posted code in your reply #26 shows a change in the X value for the last circle to be cut by 0.1mm and thus increases the diameter
of one circle from a diameter of 34.2mm to 34.6mm. Additionaly that shifts the concentricity of the two diameters such that at 12 & 6
o'clock difference between is 0.1997, at 3 o'clock 0.1, and at 9 o'clock 0.3.

Now with a 12.7mm dia cutter you figure what the finished cut diameters would be but they will not be 30.
 ??? maybe I am missing something  ???
RICH
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: Hood on July 26, 2012, 05:52:23 PM
Rich the 0.1 shift is the finish pass. So that is going round at a rad of 8.65 so dia of 17.3mm add to that the dia of the cutter (12.7mm) and the finished dia cut should be spot  on 30mm .

Hood
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: BR549 on July 26, 2012, 06:25:58 PM
I had better find my glasses. (;-)

(;-) TP
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: RICH on July 26, 2012, 09:57:36 PM
Thank you, thank you, Hood..... :)
I have tested and run a  backplotter on hundreds of files ( mill and lathe ) and never had it bomb once and on that simple one it was not interpreting the code correctly. 

Go figure......., ???
Now to get it fixed  :D
RICH
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: Hood on July 27, 2012, 02:51:39 AM
LOL no probs Rich.


Sebastian
 With the mention of your cut being 0.2 out I was just wondering if it was  when you were doing code like you posted? If you were measuring the circle cut for both the big dia and then what was left, the core so to speak?
If thats what you are doing then the core will be big dia - cutter dia - 0.2mm as you have a 0.1mm finish on the big dia.
Hood
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: s1000rr on July 27, 2012, 09:50:01 AM
It's fixed!!

So last night the first thing that I did was use the drivertest s/w to see how much I could increase the output frequency. My computer was given the green light to 100K but I decided to try 45K first and increase the step/dir to 10us. I then put my dial indicator back in place and ran the set axis one more time to see if they were still within 0.002mm and they were so I decided to make one test cut before changing to Hood's calculated settings. The circle was cut perfectly. At that point I decided to leave my step settings as they were and cut the horseshoe part, and it cut perfectly as well. I did a couple more test cuts at 10mm cut depths and higher speeds and everything always measured up so it seems my problem is fixed!!

Thanks for all the help guys, I still don't understand if it was increasing the freq to 45 or increasing the step/dir time which solved the problem but I don't want to figure that one out now that it's cutting as it should ;D

Cheers,
Sebastian
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: Hood on July 27, 2012, 01:26:42 PM
Good to hear its working, out of interest what do you have the steps per unit set to?
Hood
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: s1000rr on July 30, 2012, 11:18:55 AM
1182.change for the x-axis
1183.change for the y-axis

It doesn't make sense since they are the same pitch & belt drive but maybe since the y-axis has to move more weight (the entire table + x-axis motor mount and servo) it's steps are fractionally smaller?

Sebastian
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: derek on July 30, 2012, 12:18:27 PM
Probably a slight difference between the timing pulleys.
Title: Re: Cut parts are wrong size, CNC knee mill problem
Post by: Joel_1 on November 25, 2015, 09:25:46 PM
I am a noob having the same issue.  I will wrap my mind around this discussion and hopefully get everything calibrated.   Thanks for sharing the solution.
Cheers