Thanks Rich, I was considering that it could be a calculation error but it is translating into a large error at the machine for some reason. I will measure backlash but not sure how I could measure flex. I have tried cutting 2mm deep circles but with the same result. I was cutting the full thing out to fit into a hole as it was easier to see the error.

I know that this will probably not cure the problem but I have been looking into smooth steppers. I have also noticed that during engraving the machine is very jerky which is causing it to vibrate. Would a smooth stepper help this and possibly help my circle issue. What would be a good smooth stepper to buy and are they easy to install for a newbie?

Could there be a mismatch between my computer and the kernel speed that mach is set to? How do you determine the correct kernel speed to run at with respect to the PC?

Gary, I tried changing the setting to beziers but it made the problem worse, I got 12 flat spots rather than 4.....

Stu

Not read the whole thread so what I will suggest may already have been mentioned.
To see if it is flex you could rerun the code several times over the same point, if the circle gets better each time then that would suggest flexing of the machine is the issue. Reason being is each time you rerun it is cutting less material and thus lesss stress on the machine and less flexing.
Hood

IF CV is working "properly" AND if the 4 arc segments join correctly i.e. tangentially, then you should see no difference between 4 (90 degree) arcs and 1 (360 degree) arc because the blend between the 4 arcs should be "seamless". In that case any backlash and/or flex should produce identical results for both schemes.

If however CV is NOT working properly OR the segments do not join "properly" then you will get an "interruption" in the blend at each join which itself could cause issues but also the effects of any backlash/flex will be made more obvious.

In your gcode, the 4 arcs do appear to "join" correctly" which when added to your statement:

I have also noticed that during engraving the machine is very jerky which is causing it to vibrate.

strongly suggests to me at least that you DO have a CV problem.

Thanks stirling, How can I check that CV is working properly? As I mentioned previously I was having CV issues with rounding of 90 deg corners until I changed to using a post processor with arcs. I have tried to change CV settings to see if that made any difference but I have gone back to clearing all the CV check boxes in the config.

A bit more info that I forgot to add is that I have been speaking with someone who has an almost identical machine to mine and is also running Mach3. His machine will cut circles using arcs without a problem and he has sent me a few files which he has tested with good results at his end but do not work on my machine. Tried using Vectric to generate the G Code to make sure Artcam wasn't doing something weird but I am still having the flat spot issue.

The most annoying thing is that I know it can cut good circles just not with arcs at the moment!!

first check you actually have CV ON as you have no G64 in your code. Then maybe post your xml.

The radio button in the general config is checked for CV. I take it that it will be on by default unless otherwise instructed by the Gcode?

I will have to wait until I am next at my machine to get the xml file.

Having re-read the Mach3 install document I see that a kernel speed of 35kHz is recommended for stepper motors mine is set to 45kHz. Would that make a difference?

The radio button in the general config is checked for CV. I take it that it will be on by default unless otherwise instructed by the Gcode?

Yes.

Having re-read the Mach3 install document I see that a kernel speed of 35kHz is recommended for stepper motors mine is set to 45kHz. Would that make a difference?

Got a link? The kernel should be set to the lowest frequency that supports the max speed you require/can get. Generally speaking, with steppers, this means 25KHz. Setting the kernel to higher than needed is at best pointless and at worst likely to cause problems.

I changed the kernel speed to 25kHz and it has slowed the machine down a bit but hasn't solved the issue.

XML file attached I hope.

OK your steps/per of 127.3 and max vel of 15m/min for X&Y does indeed require a kernel of 35KHz. HOWEVER...

Your accel is pretty poor at just 500mm/s^2.

Max vel and accel are generally a trade off. Personally I'd lower your max vel and see whether you can improve your accel. CV and good accel make good bed-fellows.

You're getting different results between a full 360 and 4, 90 degree arcs. The ONLY difference I can see is that with the 4 arcs, CV HAS to do a blend whereas with a full 360 it doesn't. Given your accel is so low, I think this may be your problem (particularly with your high feedrate of 9.9m/min).

If you choose to try this then leave your kernel at 25KHz because it's sufficient for anything below 11m/min with your steps/per and I'd expect you to be reducing below even that quite dramatically to get usable accel.

BTW - you may want to revise your pin settings for e-stop.

Stirling, I did notice a distinct drop in speed when I put the kernel speed down. I should be able to bump the acceleration up a fair bit. When I was having trouble with 90deg corners I ended up putting the acceleration up to about 1200mm/s^2 to get it to cut sharp corners but seeing as I had started at 500 I thought it was a bit much. When I changed to the arc post processor I put the acceleration back to 500. I noticed that when the acceleration was at 1200 during cutting squares there was a wee bit of bounce after each corner so I suppose a safe acceleration would be about 1000? I did try a circle with the acceleration at 600 but it made no difference. I will increase the acceleration tomorrow. This may sound like a silly question but is the deceleration value the same as the acceleration value?

With respect to the e-stop pin. It was set to 10 or 11 I can't remember off hand which is the same as the Z zero plate. Every time I tried to zero the tool I got an e-stop. Someone suggested changing it to pin 2. I take it this is what you are talking about? Someone also said that I could assign pin 7 or 8  to the zero plate and leave the e-stop where it is. The first method worked and I left it for the time being until I tested other things. Should changing the zero touch plate to pin 7 or 8 work. If so I will do that as I would prefer that the e-stop system worked properly! 

Thanks very much for your help.