[FoxCNC1]

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.



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]

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]

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).

[ahren]

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

[ger21]

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]

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]

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]

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]

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]

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]

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]

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]

What does the Mach3 ATC post do differently than the other mach 3 post?

[ger21]

It allows you to output toolpaths that use different tools, and adds toolchange commands between them.

[BuckNaked31]

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]

What is G61 supposed to do? - direct step mode.
So you are suggesting I do this as a trouble shooting step?

[BuckNaked31]

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]

Thanks for sharing that. But wouldn't you want to be in xv mode when cutting circles ?

[BuckNaked31]

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]

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.