Question Undersize circles

Hi all,
Really getting to grips with my 600 – but some things are still a puzzle:

When cutting circles with my plt files - they always cut undersize. i.e. a 25mm dia circle will measure 24.7 or thereabouts.
All circles, regardless of dia are always undersize by this amount – even when using new 1mm carbide cutters (my preferred option) I get round this by using the scaling feature. i.e. recut @1.05 size

Thought this might be distortion of the Proxxon when cutting hard materials (cf) - but not sure. Any ideas?

Noticed in another post that the base Stepcraft software will cut circles as polygons –in itself probably causing slight undercutting but not convinced this is the root cause.

Which software do you use to create the file and to run the code?
Are both axes (x & y) affected?

Your article inspired me to do a test on my machine (some time this week).

Anyhow, the source of the problem could be wrong setting in machince controller or in the CAM program which generates the g-code!

Stuart Mellor wrote: ..... base Stepcraft software ....

Probably the limitations of the plt-format and/or the conversion?
http://en.wikipedia.org/wiki/HPGL

No, speedo! The limitations of the PLT format are not THAT bad.

Stuart has deviations which are 3/10th of a mm. PLT resolution is 1/40th of a mm.

I'd bet on the small set screws which are connecting stepper-motor and spindle. If these are not tightened enough you can have a backslash in this kind of dimensions.

On my machine a deviation of 2/10th also appeared recently - after one year. Have to investigate as well. My plan is to replace those small set screws with some that are a little bit longer and have a flat tip.

Thanks,
will check the set screws. Have had problems in the past with pulley screws loosening - 3 mm is not big enough - if they come loose again - will probably retap to 4mm. Its obvious if they do become loose - its an unmistakeable 'click' noise.

Really interested on other peoples tests cutting circles. Have noticed that the stepcraft software does convert the circles to polygons - which will reduce diameters slightly. Am going to measure this difference in my cad program......

Hi all,
Think I’ve got to the bottom of the undersize circle problem with Stepcraft starter software, using .plt files.
Here’s the problem – the software seems to resolve circles into polygons –thus circles will always cut undersize.

Unless – this is simply how the on screen graphics are displayed!

When the machine is cutting it’s not possible to tell if it’s cutting short polygons or not.

Using cad I have accurately measured the circles I have been cutting using 1mm bit allowing for ½ tool dia as normal ( starter software has no tool dia compensation) , inserting the relevant sided polygon inside the circle & measuring the difference in dia between it & the circle circumference.

3mm circle – is converted by the software to a 10 sided polygon. When cut the circle will be theoretically undersize by 0.1468 mm ie the max size boss which could be fitted into the hole is now 2.8532 mm!

4mm circle – a 14 sided polygon. Undersize by 0.1058 mm. Max boss size which will fit hole – 3.8952 mm

25mm circle – a 36 sided polygon. Undersize by 0.0952 mm . Max boss size – 24.9048

Since my measured errors are larger than this –t here must be another issue of slop which I’ve not yet identified.

Notice also, that the bigger the diameter – the more polygons are generated & the undersize becomes smaller.
Again I must stress – this assumes that the Stepcraft screen display is in fact the true cutting path.

Interesting!

Great analysis. Yes the PLT files have polygon limitation - but not as much geometry as you have found.


The settings will be correct for motion. You have to make the transition from motor movement through to linear movement as efficient and "slop" free as possible.

Any motor rotation that does not translate into linear motion will appear as "loss of part accuracy".

The STEPCRAFT is an open loop system - the control software moves the motors - and the machine moves. The software does not have "closed loop" and cannot check where the position is. Therefore any loss of motor-movement to linear movement cannot be accounted for.

It is therefore VERY important that all motors and drives are perfectly setup. For example - when you move the belt by hand with the machine powered off - you need change the direction of movement and watch exactly how the machine moves. as soon as the belt changes direction (simulating motor direction change) the gantry must follow.


We have our 420 going for the past year ... shes been worked hard on the standard grub screws thrugh the pulleys and they have been re-adjusted only once. You should not let all the force be taken by just the grub screw.

1) tighten the bolt agains the pulley squeezging the pulley onto the bearing untill such a point that its tight - but its not causing too much friction.

2)THEN sink the grubscrew in. With the square end of an allen key only!



the other thing to consider is the speed. If you go fast and use large cutter stickout then you will get deflection of the spindle. Cutters also "bend" too in the work. we see this with the professional machines. 3mm cutters can bend if worked too hard.



Gcode based circles are G02 and G03 commands. So the controllers run smooth pulses to the motors to machine clean circles (assuming she is mechanically sound). Non circular curves are linearly interpolated. The accuracy of this is defined in the UCCNC software - we can actually change the gain factors in the software to change the accuracy the controller operates with. YOu cannot change these values in Mach3. Don't kno about WInPC - anyone have any input her on the WinPC side?

some explanation here in video. Basically - if I was machining a flower in 3D carving - then I would loosen up the accuracy constants and let her rip. But if I want close tolerance parts - then tighten up the constants again and the speed then is related to the machines motor acceleration and speed. For most applications this is not noticed. But when you start machining in 3D or in 2D quickly then it becomes a factor.