PDA

View Full Version : Is anyone else having problem cutting circles?



FoxCNC1
03-16-2014, 01:03 PM
The machine "seems" to do well cutting rectangles pretty accurately to size. They are not 100% perfect but close enough.
However, regardless many calibrations and slowing down my already slow federate (am cutting at 20ipm) I can not get the machine to cut a perfect circle.

Let's start with why is this important?
This is important because I am making some pockets to receive a bearing. If the pocket is not perfect, I cannot press fit the bearing.

Things I have tried:

1- revised machine for loose parts
2- axis calibration over 12" and over 1/4". The machine seem to respect those calibrations on a linear path.
3- I have tried to reduce the speed of my motors ( acceleration is not set at 12) and also feed rate when cutting the circles.
4- I have tried to use a different CAM software to make the same circles

Results got better after I adjusted the step (calibration) but still not what I am expecting. #1. before, #2 after. Notice how they are taller.

http://i10.photobucket.com/albums/a146/Profoxcg/2014-03-16%2011.15.56_zps09wgzufu.jpg (http://s10.photobucket.com/user/Profoxcg/media/2014-03-16%2011.15.56_zps09wgzufu.jpg.html)

The inability to make a perfect circle happens regardless of size and its more apparent on smaller circular holes.
I am starting to think that for small parts I may need a smaller machine with smaller motors. Maybe its the electronics combo I am using.

PMDX-126 with Gecko 203 and Nema34 motors.

Attached is also the G-code. If someone with similar machine would run it and post their results I would appreciate it.
Can this really be the result of deflection, or are my electronics just unable to microstep to make circles?

ger21
03-16-2014, 01:39 PM
Can I assume that the outside corners are from a different test? The issue with those is your CV mode settings.

As for your circles.

First, you should NEVER be changing your calibration settings. Once you calibrate, and determine that the machine is cutting the correct distance (measured over a long distance), then don't change it!! Changing it will only cause it to cut the wrong length. It won't fix other issues.

Small circles are the most difficult thing to cut on a CNC. To get good results, you have to eliminate all sources of flex in the machine. What it looks like to me, is that you have flex or backlash in the up and down direction.
If you cut a 1", or 2" pocket, is it better?
Try cutting it at 10ipm. Is it better then?

With small circles, the machine needs to change direction very quickly, which can cause it to flex a lot more than most other cuts.

FoxCNC1
03-16-2014, 02:00 PM
The outside corner was cut along with the corresponding circle #1.
CV Settings are:

CV Dist. Tolerance 0.25 units. (The smaller the number the more fidelity as I understood the manual)
Stop CV on angles > 89.0




First, you should NEVER be changing your calibration settings. Once you calibrate, and determine that the machine is cutting the correct distance (measured over a long distance), then don't change it!! Changing it will only cause it to cut the wrong length. It won't fix other issues.

^ the problem I have is that if I calibrate over 24" I m afraid it won't move correctly over 1". Right now the machine is calibrated over 12" and is accurate.

If I cut a larger circle or pocket, yes it gets better. a larger circle 1" diameter will be better not perfect as you can see below.

So based on your statement of CNC machine having a hard time cutting circles, how does one accomplish a circle short of having to buy a 30K machine (which hopefully can cut a circle).

http://i10.photobucket.com/albums/a146/Profoxcg/2014-03-16%2013.54.02_zpsjkitfuov.jpg (http://s10.photobucket.com/user/Profoxcg/media/2014-03-16%2013.54.02_zpsjkitfuov.jpg.html)

ahren
03-16-2014, 02:24 PM
Cesar,

I agree with what Ger has already said -- it looks like you have some deflection in your system, and you shouldn't be adjusting calibration values. I know you have been having some difficulty with getting your gantry adjusted, and we are still planning on sending you some replacement parts to help address this per our off-line discussions. We should have everything ready towards the end of this week. I know you are eager to get going with your project and we want to help you get there as well -- we have not forgotten about you, and are hounding our specialty suppliers (mostly powder coat and heat treatment) to finish so we have parts to ship.

That being said, we often set "Stop CV on angles" lower than 89 (I have set this as low as 5). In looking at the G-code you sent, it appears your circles are broken up into 4 arc segments (which from what I understand is pretty standard, as this is compatible with multiple controllers). I would think it should be a smooth transition from arc to arc regardless of this setting, and this won't make a difference on the circles, but you could give it a try, and it should improve the corners on your rectangles.

Ahren
CNCRouterParts (http://www.cncrouterparts.com)

ger21
03-16-2014, 04:28 PM
Turn off CV Distance completely. Actually, turn off ALL CV options except stop CV on angles.


how does one accomplish a circle short of having to buy a 30K machine (which hopefully can cut a circle).

I happen to use a $150,000 router every day, and it doesn't cut round circles either. Neither did different one I used at my last job. It'll cut perfect cabinet parts at 1000ipm and full 3/4" depth, but small circles won't be round, because it has some flex in it. The flex is due to a 6 foot cantilevered gantry connected at 1 end, with over 1000 lbs hanging on it. Rapid direction changes from small circles cause it to flex.

Having said that, with a small machine like yours, you should be able to get better results.

FoxCNC1
03-16-2014, 04:30 PM
That being said, we often set "Stop CV on angles" lower than 89 (I have set this as low as 5). In looking at the G-code you sent, it appears your circles are broken up into 4 arc segments (which from what I understand is pretty standard, as this is compatible with multiple controllers). I would think it should be a smooth transition from arc to arc regardless of this setting, and this won't make a difference on the circles, but you could give it a try, and it should improve the corners on your rectangles.

I will hang on tight then.

A few comments.
regarding the "Stop CV on angles >_____" : What you are saying makes sense. Depending on application I can see someone setting it to 5 degs. Your comment made me think about this setting in more depth. I would try to maybe set it at > 39 but anything lower doesn't make much sense at least not in my case. Ideally you would want the machine to stop at sharp corners and at this time the parts I would like to make are either going to have 45 degs or 90 degs. anything else it either a circular pocket/hole, or a curve.

I will be more than happy to change the post settings of circles if that is what you are suggesting (I would need to research how to do that) and think it would make your machine and hardware run better.

Below is the other code I tried, it seems to make circles is 8 segments. Same result.
So would it be safe to say again that there is nothing wrong with the G-code generated by aspire?

ger21
03-16-2014, 04:38 PM
The stop CV on Angles setting in Mach3 is actually backwards. Setting it to 5 actually means that it will use Exact Stop mode on angles from 0 to 175°.

FoxCNC1
03-16-2014, 04:42 PM
Turn off CV Distance completely. Actually, turn off ALL CV options except stop CV on angles.



I happen to use a $150,000 router every day, and it doesn't cut round circles either. Neither did different one I used at my last job. It'll cut perfect cabinet parts at 1000ipm and full 3/4" depth, but small circles won't be round, because it has some flex in it. The flex is due to a 6 foot cantilevered gantry connected at 1 end, with over 1000 lbs hanging on it. Rapid direction changes from small circles cause it to flex.

Having said that, with a small machine like yours, you should be able to get better results.

okay, fine =)

So what we are saying here is:

1) That I am mistaken to think that I would be able to cut perfect circles on a cnc machine.
2) Because of the nature of a CNC machine, I will not be able to cut perfect circles / but since my machine is smaller (48" gantry) it should be very close. Still not perfect.

I have question, how are small metal parts (that I see everyday) that have such perfect features made?
it is a smaller machine? - do I need a "CNC MILL" ?

ger21
03-16-2014, 05:02 PM
1) That I am mistaken to think that I would be able to cut perfect circles on a cnc machine.
2) Because of the nature of a CNC machine, I will not be able to cut perfect circles / but since my machine is smaller (48" gantry) it should be very close. Still not perfect.

No, I didn't say that at all. If you get rid of the flex, you should get good circles. Your machine is probably a lot more rigid then mine, and I've cut decent bearing pockets in aluminum.

You need to find where the flex is, and eliminate it.

Frankmali17
03-16-2014, 09:17 PM
Gerry is right about the "stop CV on Angles" setting in Mach...
To me it would seem like Mach 3 setting Says "Stop CV on Angles > ____" which would mean "greater than" ____ ... but I think the sign should read the opposite " Stop CV on Angles < _____ " ... for example... when cutting a square or rectangle with 90 degree corners.. I found mach 3 running g-code and making toolpaths with rounded corners. the faster the federate, the rounder the corners I was getting.
SO I experimented. A rectangle has four 90 degree corners. A triangle perhaps would have three 60 degree corners. Therefore to cut a panel with square corners.. I figured that CV would have to be turned off at angles Less than or equal to 90 degrees. Since there is no less then or equal to setting... I set mine to 89 degrees. and it seemed to work. The tricky thing is that the way it is written, the Mach 3 setting had me confused. Anyway... setting it to 90 degrees didn't work because a rectangle is four 90 degree turns, so it would still round off corners.
Anyway, Gerry, Ahren... please comment and let me know if what I said seems to be correct.... Would it be good to send an email to Mach 3 developer about this if I am correct about the "<" sign ???

This CNCZone community, and the members of it like you guys, are awesome.

Frankmali17
03-16-2014, 09:23 PM
I agree with Ahren and Gerry,
this error seems to be more mechanically related...
On another note...
Something I learned from practice, and confirmed by others...
Cutting or pocketing using climb cutting, yields smaller pockets, then when you cut the pocket conventionally.
For example.. when cutting out and inside profile or pocket, the climb cutting technique causes the cutting tool to deflect away from the material... when you cut conventionally, the tool wants to bite into the material.. pulling itself into the profile, and it yields a slightly larger pocket then you intended...
My machine is a DIY with a lot of wood parts, but also aluminum V groove profiles, and V groove bearings... and I am learning a lot from it before I build some serious metal... :-) Right now, Ahren's kits are in my sights ;-)

ger21
03-16-2014, 10:22 PM
Would it be good to send an email to Mach 3 developer about this if I am correct about the "<" sign ???

They've been made aware of it many times I'm sure. It's unlikely imo that any more development will ever be done on Mach3. Mach3 was at the point where every time one bug was fixed, at least one more was introduced. It got too complex for it's own good.

The developers have been working on Mach4 for several years now, and claim it will be finished soon. But, they've been saying that for years too.

FoxCNC1
03-16-2014, 11:28 PM
What does the Mach3 ATC post do differently than the other mach 3 post?

ger21
03-17-2014, 07:42 AM
It allows you to output toolpaths that use different tools, and adds toolchange commands between them.

BuckNaked31
03-18-2014, 02:16 AM
All you have to do is insert a G61 before the circle. If it still doesn't cut right, it's not the CV settings. I switch back and forth all the time for various operations. Just don't forget to put it back into CV mode with a G64 when you are done cutting the circles.

Sent from my SCH-R720 using Tapatalk 2

FoxCNC1
03-18-2014, 07:19 AM
What is G61 supposed to do? - direct step mode.
So you are suggesting I do this as a trouble shooting step?

BuckNaked31
03-18-2014, 08:01 AM
You can do this any time you want to move out of cv mode, whether you are troubleshooting or not. It's there for a reason. I use it as a tool in programming. It works well. It's exact stop mode, btw.

Sent from my SCH-R720 using Tapatalk 2

FoxCNC1
03-18-2014, 08:07 AM
Thanks for sharing that. But wouldn't you want to be in xv mode when cutting circles ?

BuckNaked31
03-18-2014, 08:22 AM
If you want the best precision, cv mode is not the way to do it. The reason why I said it is that all this talk a few posts back about changing Mach's config to trace down a problem with CV was a lot of work considering all you needed to bypass it was a G61. Now, the other issue of using G61 or G64 when cutting circles... CV mode itself is a compromise between speed and accuracy. It alters the path, period. G61 does not. If you are wanting the cut as perfect a circle as you can, use G61. If you want to cut it fast, use G64. You ain't gonna get both :)

Sent from my SCH-R720 using Tapatalk 2

LeeWay
03-18-2014, 08:36 AM
The key is to have a machine that does not flex. Everything else is a work around. It takes extra effort to make a less optimal machine to cut everything well. That is one of the trade offs. My home made 80/20 mill does a fair job milling even circles. It does so at the cost of higher tool breakage simply because the spindle is not as rigid as it needs to be.
I can tell when the bearings are starting to get loose by increased tool consumption. The spindle (X2 head) is the weak link. Your cnc router will only be as strong as it's weakest link. Right now, it looks like you may have flex in the Z axis. Steps taken toward correcting that will get you better results than adding Gcode work around, however they will work fine short term.
Mach 3 also has a backlash compensation tool. I haven't needed it, but some have used it with good results. IE Hoss.

BuckNaked31
03-18-2014, 08:42 AM
I would hardly call changing from CV to exact stop a "workaround." I do however agree with you on the flex issue. See my last post, I've added to it since yours...

Sent from my SCH-R720 using Tapatalk 2

LeeWay
03-18-2014, 08:49 AM
I simply meant that with a rigid machine, you do not have to fuss with the CV settings or Gcode. If you do have to mess with it, it is a work around. That is unless you update the post processor in your CAM package to handle it every time. That said, the action of modifying the PP is a work around. ;)

That wasn't actually the point of my post though. Rather than a work around, lets call it less optimal. :)

BuckNaked31
03-18-2014, 09:03 AM
I hear you, but unless you or anyone else can get a motor to instantly accelerate, isn't it all a "workaround?" :)

Sent from my SCH-R720 using Tapatalk 2

BuckNaked31
03-18-2014, 09:08 AM
Btw, you don't have to modify your PP to do it... I just edit the file and insert it. Kinda old school, I guess...

Sent from my SCH-R720 using Tapatalk 2

LeeWay
03-18-2014, 09:10 AM
Getting someone else to machine and ship you parts for less than you can make them for is ideal for me. That is optimal. :) That is what I have going on with one of my suppliers currently and I could not be happier. It is like hiring another guy without having to pay his insurance. :)

That is definitely getting around work. ;)

BuckNaked31
03-18-2014, 09:27 AM
Sounds like you've got it all figured out. I build guitars, but someday I would like to have someone working at the shop while I drive around and buy cool looking wood. It's a dream for sure. For now I'm stuck programming for machine shop and building guitar parts in my spare time...

Sent from my SCH-R720 using Tapatalk 2

LeeWay
03-18-2014, 09:38 AM
I started part time in 03. Stick with it. I still don't have time to do much woodworking, but I can buy nice wood when I see it. :)

All figured out? Not hardly. Maybe next week. ;)

knightsofnii
03-19-2014, 10:27 AM
use the drill function, and use the bit the size hole you need. for small holes anyway.

FoxCNC1
03-19-2014, 07:00 PM
^ I just need to get the machine some rigidity as mentioned and go from there. I will try the direct mode and cut some circles.
But as stated before, I agree that everything would be a workaround until I upgrade / "fix" the machine.

I appreciate all the help and CNCRouterparts is behind their product all the way which I am happy about.

ger21
03-19-2014, 10:18 PM
If you are wanting the cut as perfect a circle as you can, use G61. If you want to cut it fast, use G64. You ain't gonna get both

If the circle code is a single G2 or G3, they'd both cut exactly the same.
However, since his g-code is cutting with 4 arcs, G64 would be preferable imo. With G61, his code will stop 4 times as it cuts the circle, magnifying any flex he has. G64 will cut the 4 arcs as one continuous circle.

Arcs and circles are not normally an issue with CV mode. Code made up of short straight segments or sharp corners can cause issues.

BuckNaked31
03-19-2014, 11:27 PM
If his CV settings are out of whack with his motor acceleration settings, they will cut sloppy. This isn't hard to do with Mach. But the reason why I said what I said was because someone was telling him to make all kinds of changes to his settings to test, when all he had to do was put a G61 in his code and cut circles for test purposes. I would agree with you totally if the circles he was trying to cut were bigger, but they are tiny. I would agree that flex may be an issue, but it's more than likely that something is loose somewhere. I highly doubt that given the fact that he's using a CNCRP setup, he actually has a flex problem... Unless we're referring to something being loose as flex. Those machines are more than stiff enough to cut a good circle.

Sent from my SCH-R720 using Tapatalk 2

FoxCNC1
03-19-2014, 11:42 PM
I value both of your input. I you are right, there all kind of flexing things. My gantry risers have some play in them, I tighten the motor and it helped a bit.
I cut a 1.5" circle pocket and it came out pretty well. Much better than this weekend.

I read somewhere about the "pull test" I engaged the motors (power on the machine) and started to tug at it. And I noticed there more play on the risers than on my Z carriers and Z axis.

Once I tried to tighten everything (Still some play left) I run a circle pocket. I also used HSM express (I am an inventor user) to make the G-code and the results were quite acceptable. I really bought is the G-code that made the different.

I just really need to get my upgrades and loctite all the bolts.

Here is a pic.

http://i10.photobucket.com/albums/a146/Profoxcg/20140319_233516_zpssx73s0pg.jpg (http://s10.photobucket.com/user/Profoxcg/media/20140319_233516_zpssx73s0pg.jpg.html)

BuckNaked31
03-19-2014, 11:46 PM
I'm glad you're getting it straightened out. Good luck! When you start getting some projects cut, post some pics :)

Sent from my SCH-R720 using Tapatalk 2

FoxCNC1
03-19-2014, 11:49 PM
You have no idea how much I want that BuckN. I have been sturggling with this machine / learning through hard knocks since Nov 2013. I have yet to cut anything "real" But I know that with the support from you guys and CNCRP I will be up a running in no time.

diyengineer
05-10-2014, 10:33 PM
More than one way to shine a turd. Make a rough cut and come back with multiple finish passes so it will deflect less. Use a shorter tool, buy quality tooling, and know the limits of your diy machine when programming.


Washington state

FoxCNC1
05-10-2014, 11:26 PM
Thanks, it's all sorted out.

diyengineer
05-10-2014, 11:27 PM
Good to hear!


Washington state

jonmessenger
11-03-2015, 05:20 PM
I've been reading through this thread, and i hate to tell all the "Flex in Machine" Guys that you may be wrong, but "You May Be wrong" you see i have always had this problem as well, and i thought is was that, but i just completed a Plasma Cutter and guess what? you got it oblong circles. the plasma cutter never touches anything. i think it might have something to do with the way mach interprets I s and J s in mach.

No solution yet

xjdubber
11-03-2015, 07:33 PM
I've been reading through this thread, and i hate to tell all the "Flex in Machine" Guys that you may be wrong, but "You May Be wrong" you see i have always had this problem as well, and i thought is was that, but i just completed a Plasma Cutter and guess what? you got it oblong circles. the plasma cutter never touches anything. i think it might have something to do with the way mach interprets I s and J s in mach.

No solution yet

This is not a problem with Mach whatsoever if your circles are coming out oblong, you either have not calibrated your x and y correctly of you have backlash issues.

LeeWay
11-03-2015, 08:01 PM
Calibration does mean a lot on some machines. You cannot just punch in the numbers that should be there after doing the math. You need to actually measure the travel to confirm or adjust the steps to get the target length. Mach 3 has a calibration aid for adjusting the steps per inch or MM and it will let you dial each axis in. Once you know that the machine travels 5.75" when you call for that distance, then you are farther along in troubleshooting the cause. You may find that the issue disappears.
On a plasma, just because the torch isn't inducing any cutting forces into the machine, doesn't mean that all the other axes aren't either. Especially given the speed needed for some materials. A gantry traveling at 150 IPM may suddenly need to go back where it was coming from. It has to stop all that momentum instantly. Any slack at all will show itself right there. Consider how many times the machine may do that during a job. Mach 3 does try and lessen that type of impact with CV.

knightsofnii
11-04-2015, 10:48 AM
I have had shape and curve problems from a couple things:

1: the set screws spun out of my pinion gears, causing the x axis to "studder", most notably after switching directions. That took a long time then a eureka moment to find.

2: I imported .stl 3d shape from one cad software into Aspire, and the shape changed a pinch.

3: on shapes with curves, the CAD software I have created different line thicknesses for different curves. Now I always make sure I set my line thicknesses to 1 pixel, and then when in my cam software I convert polylines to splines (which also can skew things a pinch).
this way, the machine doesn't get confused which parts of curves are starts and ends, therefore making it cut on different sides of a line, or if cutting on the outside or inside of lines of different thickness, not producing squiggles.

After "fixing" 1-3, I have really nice shapes.

Jon.N.CNC
11-04-2015, 12:30 PM
Calibration does mean a lot on some machines. You cannot just punch in the numbers that should be there after doing the math. You need to actually measure the travel to confirm or adjust the steps to get the target length. Mach 3 has a calibration aid for adjusting the steps per inch or MM and it will let you dial each axis in. Once you know that the machine travels 5.75" when you call for that distance, then you are farther along in troubleshooting the cause. You may find that the issue disappears.
On a plasma, just because the torch isn't inducing any cutting forces into the machine, doesn't mean that all the other axes aren't either. Especially given the speed needed for some materials. A gantry traveling at 150 IPM may suddenly need to go back where it was coming from. It has to stop all that momentum instantly. Any slack at all will show itself right there. Consider how many times the machine may do that during a job. Mach 3 does try and lessen that type of impact with CV.

Ive always found the axis calibration to be less effective than a calculator, mostly because it does not calculate to enough decimal places. To calibrate better I simply work out the steps per mathematically. Place a dti at one extent of axis travel, and run the axis from - extent to the dti, if it's off I simply add or subtract step units incrementally from the end decimal places and repeat until it is within the desired accuracy.

It's the only way to get it spot on imo, re entering the travel into the axis calculation will loose you decimal places of accuracy, you want it to around 9-10 decimal places.

LeeWay
11-04-2015, 12:44 PM
Mach 3 gets pretty deep in the decimal point. I often thought that was overkil, so I always rounded them up to 4 points.
It has to be repeated many times in several locations on the axis, but it you get you very close if you stick with t. I also recorded each step change, so I could average them all out across the length of travel..

Jon.N.CNC
11-04-2015, 01:22 PM
Mach 3 gets pretty deep in the decimal point. I often thought that was overkil, so I always rounded them up to 4 points.
It has to be repeated many times in several locations on the axis, but it you get you very close if you stick with t. I also recorded each step change, so I could average them all out across the length of travel..

I think Mach 3 goes to 6-7 decimal places.

Just 4? That's either very coincidental that you have accuracy with just 4 decimal places or your not as accurate as you think you are.

Obviously due to steps being exponential, on smaller machines you can calculate to large number of decimal places but will be accurate with less. On an 8x4 machine over 2440mm a change at 9 decimal places does register on a dti.

Wtf Sorry can not does, if I try to edit this forum deletes my last paragraph :s infact it's deleted this paragraph twice now when I have entered the last paragraph.

With mine i am lucky to be within 1mm with over full 8ft of travel with the inbuilt calibration, with a calculator and repeatedly making manual changes I get within 0.05mm which is the mechanical accuracy of the machine.

O and it's deleted it anyway, I have to type again :s

But you kind of already confirmed that by saying you have to repeat multiple times, you really shouldn't need to, sounds like your just retrying until you get lucky.

With a calculator you should be within 0-0.15mm instantly.

Jon.N.CNC
11-04-2015, 01:47 PM
I think Mach 3 goes to 6-7 decimal places.

Just 4? That's either very coincidental that you have accuracy with just 4 decimal places or your not as accurate as you think you are.

Obviously due to steps being exponential, on smaller machines you can calculate to large number of decimal places but will be accurate with less. On an 8x4 machine over 2440mm a change at 9 decimal places does register on a dti.

Wtf Sorry can not does, if I try to edit this forum deletes my last paragraph :s infact it's deleted this paragraph twice now when I have entered the last paragraph.

With mine i am lucky to be within 1mm with over full 8ft of travel with the inbuilt calibration, with a calculator and repeatedly making manual changes I get within 0.05mm.

O and it's deleted it anyway, I have to type again :s

But you kind of already confirmed that by saying you have to repeat multiple times, you really shouldn't need to, sounds like your just retrying until you get lucky.

Sorry this forum started to spin me out then, it seems to be buggy in safari.

LeeWay
11-04-2015, 02:06 PM
No. I repeat multiple times along the axis in different locations. Then average them out. I was mainly talking about mils with short axis travels generally. Longest being maybe 14". You can log deeper decimal places if you choose to of course. I do not have any equipment that would measure any closer than 4. :)
For my bigger plasma cutter, I just went with whatever Mach gave me. Only did it a couple times on each axis. It has rack and pinion and X and Y.
I will dial it in closer on my new CNC router parts machine though. It has R&P too, but I will be looking for a little better accuracy across the board than I set up for on the plasma.

Jon.N.CNC
11-04-2015, 02:16 PM
No. I repeat multiple times along the axis in different locations. Then average them out. I was mainly talking about mils with short axis travels generally. Longest being maybe 14". You can log deeper decimal places if you choose to of course. I do not have any equipment that would measure any closer than 4. :)
For my bigger plasma cutter, I just went with whatever Mach gave me. Only did it a couple times on each axis. It has rack and pinion and X and Y.
I will dial it in closer on my new CNC router parts machine though. It has R&P too, but I will be looking for a little better accuracy across the board than I set up for on the plasma.

Try the manual way, I too used to do it a similar way to you but it just never seemed to be right with poor repeatability. One way to test on a smaller machine is to make up a program that starts a minus extent travels to positive extent into dti and back again and repeat 50 times, just monitor the dti for a drift will tell you how accurate you are.

The more decimal places you have the better chance you stand at the test being repeatbly accurate. Preferably all the decimal places of the mathematical calculation or maximum software denomination.

LeeWay
11-04-2015, 02:41 PM
I would need better instruments. :)
Mach 3 is only going by what I have told it that the machine actually moved. I get that number from my dial indicator. It only read s 4 decimal points, but I would not count on that forth one. Unless it is a Starrett Or Mitutoyo or something. Mine aren't.
I bought a Starrett dial indicator once. Next time I went to use it, it was in pieces. If I could have laid my hands on No body, I would have. Apparently No body did it. ;)

dgage
11-04-2015, 03:39 PM
Can someone point me to some info on this DTI and multiple axes? I'm not familiar with DTI and the only thing I really found looking up "CNC DTI" was a video on Youtube checking height with a dial indicator over multiple points on the table. Not sure how I'd do something like that for the X or Y axes to get to 1 digit much less 6 or 7 digits of accuracy. Thanks.

Jon.N.CNC
11-04-2015, 03:51 PM
I would need better instruments. :)
Mach 3 is only going by what I have told it that the machine actually moved. I get that number from my dial indicator. It only read s 4 decimal points, but I would not count on that forth one. Unless it is a Starrett Or Mitutoyo or something. Mine aren't.
I bought a Starrett dial indicator once. Next time I went to use it, it was in pieces. If I could have laid my hands on No body, I would have. Apparently No body did it. ;)

.4 decimal points is plenty your machine will only be accurate to two.
A decimal point in steps per is not a decimal point of a mm unless your machine does 1mm per step. In which case the accuracy would be horrendous.

It's a repeatable accuracy your looking for so with a program such as the one one I mentioned, if your accuracy is out the drift will be exponential Ie one travel is out .001mm per step over 100 steps it's out 0.1

So you want to set the dti up at the furthest possible travel and start at the furthest opposite extent, you want to be measuring as many steps as possible.

If it's accurate to 4 decimal places over the entire axis travel then you must have some next generation machine as mechanically the best screws you can get are only accurate to 0.012mm.

And you won't get enough decimal places of measure with any instrument if you are say stepping one mm into a dti and using the measurement. This is again why a mathematical calculation is more accurate.

Sounds as maybe you are getting slightly confused between a backlash test and a steps per calculation.

ger21
11-04-2015, 06:19 PM
.4 decimal points is plenty your machine will only be accurate to two.

Maybe for you metric guys, but not here in the US. ;)

LeeWay
11-04-2015, 07:15 PM
Yep. Even the backlash on my rolled ball screw is in the low third decimal point. And it's a cheap screw. :)

I do get what you are saying about the step count being different from distance traveled. They are different.I used the method I mentioned on my home made mill. It has some nice NSK ground ball screws on it. They were preloaded with two different size balls.
That all helps to lessen any backlash.
My parts do not need high tolerance accuracy, but when I did machine stuff in testing, they came out to the exact final dimensions I was shooting for. I would have to take into account the actual end mill size and do a finish and spring pass, but hey, it preformed accurately at least as far as I could measure. Not bad for a home made machine. :)

diyengineer
03-04-2016, 05:34 PM
Another thing you can do with small holes is either choose to drill them, drill and followup with boring them, spot drill them and followup by hand drilling them, drill them under size and followup with a router bit, or endmill to clean up excess with a lighter cut.

Rathkamp-Drums
04-22-2017, 06:07 PM
This has been an interesting read. It's even more interesting that backlash is only briefly mentioned. To interpolate a circle, both the X and Y axis change directions.

In a production machining environment, circular interpolation is NEVER used to achieve a finish size in a hole with a tight tolerance.

You can often tune some of this backlash out, but it will never be perfect.