I was running with routers so far . Sure Mach3 is very useful for the routers.  Now I've  built a laser table and now trying to setup it now. My problem is the lines or splines etc are not smooth. Laser causes the errors are seen clear since the kerf is too thin . First I have used steppers driving by Geckos with 10 microstep . Resolution was around  0.1 mm. Unfortunately I 've get terrible results . I'was not expecting such a bad result. Lines, curves were too rough. Then I have converted the table drives to high resolution servo drives. Now Results are better but not as good as it should be. Now resolution is 0.02 mm. I guess the main reason to get rough finish  is not only the low resolution. Mach 3 gives pulses rough.
 Awaiting your comments  

A resolution of 0.02mm should be plenty, I presume your code is a straight line G code move, not lots of little moves?
Also is the motion of the table/gantry smooth. Is it a diy build, hows the table driven etc.
For example if the gantry is a slightly flexible and the linear slides have a bit of stick, with a centre lead screw you can get a motion that's kind of wobbly as first one side moves and sticks while the other side is doing the same out of time with each other.
Sorry if my explination is a little rubbish but I can't think how to put it into words.

Thinking about it with a resolution of 0.1mm on steppers you must have cables of tooth belt drives each side of X which would stop this happening.

Steve

This is DIY cnc laser table. Tube is chinese 80 W ones. Gantry is driven both sides to keep the motion equal both sides. I have used T5 type gears and toothed belts. I'm thinking if I should use MXL types since they are running smoother. But I still think Mach3 is the main factor. Manual jogging running smooth but when the program running I see some jerky movements. Particularly if the feed rate is not 100%  jerky movements  become more visible. I wonder If I use smooth stepper can I solve the issue.

Can you attach a bit of your code where you have erratic running?

I'm using  Z 2,5D option to on/off the laser. For this  reason I keep the  Z  +0,1 - 0,1 mm range to save time.

Hi

I've only quickly looked at the code but a fair amount of the lines of code are X then Y moves rather than X & Y together, this would create the stair stepping that your talking about, some of the moves are both together however.

I'll have a look at it in mach later but can you cut a diamond shape or triangle with g01 moves, say something like

G01 X20Y30 F1000
G01 X30Y20
G01 X20Y10
G01 X10Y20
G01 X20Y30

and see if this produces smooth flat sides.

Steve

I looked at the toolpath on one of the ribs in the bottom of the drawing. The outside profile consists of many short simultaneous straight/linear movements of the x and y axis instead of longer arcs segments. Your feedrate is high. I got 1800mm/m. That is 70.8 ipm. Is that correct?

With such a high feedrate and short lines instead of longer arcs you can/will get rough running if you have chosen exact stop in the general configuration menu. Have you exact stop or constant velocity checked? Next is your CV Distance led/button on the Settings page should be on. Is it? What value has it? If on and Zero value it is the same as exact stop even if you have constant velocity in your configuration menu. Also the constant velocity button may cause it. Is it on? what value has it?

Nice work though. What plane is it for? What scale is it?

Most of the time it is not possible to create the shapes as an arc form. Once exploded circles are turned to small llines . unfortunately it is not possible to keep the circles as an arc again.(at least I don't know ) I have chosen high feedrate since it is cut by laser. I have chosen constant velocity mode . For smaller objects  exact stop mode gives better results as expected.
" Next is your CV Distance led/button on the Settings page should be on. Is it?"
 As far as I know just checking it in genaral configuration menu is enough. I've never checked it in setting page so far. it is on and value is 180 but CV feedrate led is off.  What is CV feedrate ?

"I'll have a look at it in mach later but can you cut a diamond shape or triangle with g01 moves"
  Sure I will cut it.

 By the way it is 50 cc yak wing..

What is CV feedrate ?

CV feedrate is, as I have found, the maximum allowed feedrate in "corner cutting mode", that is in the exact parts of the cutting where CV feedrate/CV distance is working. CV feedrate is working at the end and beginning of line and arcs segments.

CV distance is how far from the start and end of a line or arcs segment where "corner cutting" is allowed. A high value or not turned on gives deviation from the original toolpath on a relatively long section at the intersection of two line or arcs segments. A low value gives a short distance where the actual toolpath deviates from the original toolpath, but at the same time lower feedrate in those same sections.

You may want to set the CV distance to a low value like 0.1 to 0.3 when you need reasonably sharp corners. Such a low CV distance value gives nearly as sharp corners as exact stop mode but still considerably higher feedrate. When more rounded corners is allowed a higher value like 0.5 to 2.0 may be adequate. A CV distance of 180 gives very large deviations from the original toolpath when the feedrate is high and/or acceleration is low.