CV or ES setting in Mach3 - (Constant Velocity or Exact Stop)
 

I was playing with the exact stop vs constant velocity settings and was getting very different results. With the default setting of cv (180) my parts corners were excessively rounded at 500ipm I initially though it was lost steps but there was no lock up and returned exactly to home. When I changed to exact stop the parts came out great at the same 500ipm. I am looking to cut as fast as possible for production work, can anyone with some experience in these settings lend me your advice? I did look at the Machsupport forum which suggested changing the cv values to .01-.03 for sharp corners and .5-2.0 for slightly rounded. I will give this a try but seems so far from the default settings. Also, suggested that I change settings under tangential control (lift angle to 0.) It is my understanding that some cam programs change between cv and es. I am using cut2d and will have to see if it does this in the code. Is cv directly related to motor acceleration and look ahead? My best guess so far is that for high feed speeds acceleration is set to max and cv is set to what is acceptable on your parts corners and how much jerk your machine can handle.

How fast can the Mechmate cut OSB and Plywood with acceptable results? This question is going to very greatly depending on the PC, Motors, power supply, pinion gear, bits, depth of cut, router or spindle, acceptable part quality, settings in Mach3, 2d or 3d cutting, etc.

Anyone been down this road all ready?

Justin

What CAM software are you using? You can make some adjustment there also.

I have to look at my Mach setting to see what I currently have.

I think this is a very good topic. Thanks for starting a thread.

Hi Nils, I think you are also using Vectric CAM..If so where and how do you adjust it there.

Nils,

I am using Cut2D from Vectrics.

I am using Aspire.

Thought so, but I would imagine it will be more or less the same in V-Carve pro as they are from the same company.

Strangley enough - I have been dealing with the same thing - I did find a setting in Mach - that allows you the specify what angle that Mach will switch to exact stop - I have mine set for 90 degrees. Still determining myself if thats helping or not. I'm using vectric products as well.

(BTW folks - I'm making dust :) )

When in CV mode, corner rounding is maily determined by acceleration. The faster the accel, the less rounding will occur.

Say you're traveling along the X axis and want to make a 90 degree turn. In order to maintain a constant velocity, as you get near the corner, the X axis will begin to decelerate. At the same time, the Y axis needs to start accelerating. This rounds the corner.

There's a CV manual here.
http://www.machsupport.com/docs/Mach3_CVSettings_v2.pdf

I cannot find the place where these settings are changed and Mach frustrates me terribly . . . .

Deleted - out of date

Gerald,

I am using Version R3.042.020 (Config) (General Config) (Motion Control) (CV control).

Okay, the release at that computer was a bit old. Here is what is seen with current Mach releases:

Hi Gerald and crew,
I am also wrestling with this one on my new purpose built cnc. I am used to shopbot, and mach3 seems very arcane and hard to understand on this issue, though Art's explanations seem straightforward enough. As far as I can work out the cv distance tollerance is a critcal setting, as it dictates the distance from the sharp turn that rounding can begin. If you draw it out in cad, if it is set to 1mm, with a 6mm cutter, then at a turn above 30 deg, it has no rounding effect on inside corners, and at lower turn angles the rounding is not noticable. The default setting of 180 is obviously set for no limit, or maybe to cover the issue if your units are steps. This works ok, but I don't know if there is a way of adjusting this figure from gcode, so I can set it for different cutter diameters from software. Also do I need to set a cv angle limit to prevent lost steps at 90 or 120 deg bends? Finally, the machine is often stopping when the path comes to curve that starts off in line. I have the lookahead setting at 20 lines, and most of my programs are not much longer than that. What do I need to look at for that?
I have combed the mach3 forum, and all I find is confusion, as the names, position and parameters of the settings seem to change between versions.
Best wishes, Ralph

I had the same problem, but when I checked the 'stop CV on angles' and entered a angle of less that 22.5 degrees then the software would slow down the travel so as not to create a round corner. Can't remember if I had to adjust anything else?

An important setting that does not get much coverage is the CV Feedrate on the settings page, make it the same as the fastest feedrate in your current running file, makes a HUGE difference to how the machine performs when going from line to line. My machine was having a small pause at the end of every line, even if the following line was straight and in the same direction (with CV set on, Dist tolerance 0.9 units and stop CV angle >90 deg), With the CV feedrate set at +1 (the default) performance was appaling, set to 2500 (my standard feedrate, mm's) the machine is smooth and flies along from sector to sector.

Thanks, I'll play with that, R

-
 

We would like to set the "Region" column to display the South region first followed by North.
I understand we can click on the Region column and has it in ascending order or descending but it there a way to set it for all users to show South Region customers first followed by North Region Customers.

Thank you,
Kendra