[curacao]

Hello all,


I have a problem with my MK3/CNC USB Controller settings. When I try to cut a test file [basically a star] it does not cut the entire shape in one smooth motion. It stops in every corner. In simple shapes it is less of an issue but I tried to cut a tree design where its made of many lines and the plasma torch shakes instead of moving fluidly.

a college suggested I look at the "lookahead" settings. I have messed around with them and tried it ever times and noticed no real change. Here are the settings I am currently using.


Here are my settings file [CNC USB Controller]:
https://drive.google.com/file/d/0B_q...ew?usp=sharing

Here is the G-Code I was trying to cut:
https://drive.google.com/file/d/0B_q...ew?usp=sharing


If anyone also has suggestions for settings I should change specifically for plasma cutting. Please let me know.

[robertspark]

Hello all,


I have a problem with my MK3/CNC USB Controller settings. When I try to cut a test file [basically a star] it does not cut the entire shape in one smooth motion. It stops in every corner. In simple shapes it is less of an issue but I tried to cut a tree design where its made of many lines and the plasma torch shakes instead of moving fluidly.

a college suggested I look at the "lookahead" settings. I have messed around with them and tried it ever times and noticed no real change. Here are the settings I am currently using.


Here are my settings file [CNC USB Controller]:
https://drive.google.com/file/d/0B_q...ew?usp=sharing

Here is the G-Code I was trying to cut:
https://drive.google.com/file/d/0B_q...ew?usp=sharing


If anyone also has suggestions for settings I should change specifically for plasma cutting. Please let me know.

I don't use planetCNC, but it sounds like you are running in exact stop mode and not constant velocity

[PlanetCNC]

Set "Angle" to 165, "Radial Acceleration" to 80, "Path Tolerance" to 3.
Make sure you use G64 and not G61,

[curacao]

Set "Angle" to 165, "Radial Acceleration" to 80, "Path Tolerance" to 3.
Make sure you use G64 and not G61,

Hello,

In my talk with [email protected] they told me to switch to PlanetCNC TNG software. Now I am trying to figure out why my plasma is stuttering. The new software has no manual.

Here is a picture of a cut.


It is annoying that I have to wait for a response every time. I wish there was a clear manual that explained how to set everything up. Because I am on the other side of the planet, every time I have to wait for a reply its a day I lost and cannot cut.

[robertspark]

I can't help myself, (as I know zero about planetcnc but have to ask)

Are these settings in inches or mm?

<Axis1>X</Axis1>
<Axis2>Y</Axis2>
<Axis3>Z</Axis3>

<Axis1StepsPerUnit>106.838</Axis1StepsPerUnit>
<Axis2StepsPerUnit>106.838</Axis2StepsPerUnit>
<Axis3StepsPerUnit>1086.957</Axis3StepsPerUnit>

<Axis1MaxSpeed>4000</Axis1MaxSpeed>
<Axis2MaxSpeed>4000</Axis2MaxSpeed>
<Axis3MaxSpeed>500</Axis3MaxSpeed>

<Axis1Acceleration>100</Axis1Acceleration>
<Axis2Acceleration>100</Axis2Acceleration>
<Axis3Acceleration>20</Axis3Acceleration>

If in inches, the units per step looks very course, and the maximum velocity setting of 4000 inches / min looks very high.
If in metric / mm, the acceleration looks very low for plasma cutting, your z axis has a lot of steps per unit (especially if you plan to use THC at some point), the X an Y are a bit fine in my opinion for plasma cutting (1 step per 0.009mm)

(what does the back side of the cut look like?, is there a lot of dross?)

I noticed in the screenshot below that PlantCNC has a "acceleration >> radial acceleration" setting, is this the same as centripetal acceleration?

Rob

[PlanetCNC]

Values in our settings file are in millimeters. Acceleration is in mm/s^2 (not minutes) speeds are in mm/minute. "radial acceleration" setting,is same as centripetal acceleration. curacao uses TNG now and our new software (TNG) does not use this setting any more. He also uses THC and he says it works fine..

I ran his g-code with his settings on one of our test machines and all motion was smooth as it should be.


PS
This thread looks like we are ignorant about this case. This is not true. We are helping this customer through our support system. I was up all night trying to find solution :-)

[robertspark]

No, I don't think that it reads PlanetCNC are ignorant of the issue, customers always want an issue sorted yesterday, in fact they just don't want the issue...

I've come from Mach3, dabbled in Mach4 and now use UCCNC, I did consider PlanetCNC when I was looking for something better than Mach3.

Could you explain to me what the "TNG" means and does differently (I use sheetcam TNG, but never considered that the TNG was or meant)?

With UCCNC, the values are considered as units, i.e. they could be inches or mm or apples if you desire... (does it really matter as long as its steps per unit, units per time etc).

The feedrates look correct in MM (a little low on the maximum velocity for plasma cutting potentially, depends what amperage your machine is and what material + thickness you are cutting)

The acceleration looks VERY low.... for plasma cutting, the number that gets quoted as a design target is 0.3g (9810mm/s/s x 0.3 = 2943 mm/sec/sec) or close as possible.

The problem with plasma cutting is you require constant velocity, and you require near constant velocity when changing direction, if you spend too long in one place you will get overburn and uneven cut.

Trust me I know how difficult 0.3G acceleration is to achieve

But from the numbers extracted from the settings profile, the X&Y acceleration is 106.838 mm/s/s (i.e. ~0.01G) very very low, so it will take your machine a long time to achieve it's desired feedrate.

Set aside the maximum velocity for a minute as this if not normally what you cut at, and really you only need to maximum velocity to equal the highest cutting feedrate you will require because of the amperage of your machine, material type and material thickness.

Looking at your gcode file, you have a cutting feedrate of 3700mm/min (61.66r mm/sec), at your acceleration of 106.838mm/s/s, it will accelerate to full feedrate in 0.5772 Sec, but the distance to accelerate to full velocity will be 17.8mm

With a centripetal acceleration of 106.838mm/sec/sec (which is the quickest you could possibly have given one axis will be slowing down and the other accelerating), then at the same feedrate 3700mm/min, the minimum radius you could cut would be 35.6mm radius....

Also looking at your gcode, "normally" on small acs and circles (less than 25mm dia), the advice is to slow the feedrate down to about 60% of the quoted / target linear feedrate, hence I would expect to see in your gcode a Feedrate of about 2220mm/min on all G02 + G03 motion (if it's less than 25mm dia), and a feedrate of 3700 inserted after the next linear move after the G02 + G03 motion {note there is also the option to slow down and speed up a certain distance before corners which is also advocated with plasma on thick plate, but that is another discussion).

I additionally noted within your gcode that you have:

N0120 M03
N0130 G04 P0.4
N0140 G01 X215.3143 Y246.9743 Z1.5000 F1500.0
N0150 G02 X218.5930 Y245.4389 I0.8716 J-2.4070 F3700.0

N120, turns the torch on
N130, waits for the pierce delay 0.4 Seconds??
N140 moves both the X,Y and Z axis at a feedrate of 1500mm/min.

"normally" with plasma cutting, once the torch fires, it waits for the ArcOK (transfer) signal to be recieved, then waits for the metal to pierce, then decends to the cutting height (as fast as possible, given if you spend too long getting there the kerf will get bigger as the torch has more time to cut, arc to wander and molten metal to be blown out of the kerf), and then X + Y motion begins.

Hence I would have expected the post processor to do something like this:
N0120 M03
N0130 G04 P0.4
N0140 G00 Z1.5 (rapid move to cut height)
N0150 G01 X215.3143 Y246.9743 F3700.0
N0160 G02 X218.5930 Y245.4389 I0.8716 J-2.4070 F2220.0
....

normally in sheetcam the

N0120 M03
N0130 G04 P0.4
N0130 G00 Z1.5 (rapid move to cut height)

is done within the "pendown()" function for the sheetcam post processor


You would also then add

N1010 M05
N1020 G00 Z20.0000


to the "OnPenUp()" function within the sheetcam post processor.

to make this happen correctly you would need to edit the post processor and possibly remove the Z axis motion from the OnRapid(), OnMove() and OnArc() functions within the post processor.

[PlanetCNC]

TNG stands for "The New Generation". I know this from Star Trek:-)

PlanetCNC also uses "units", probably same as UCCNC. You can set in which units you want user interface, which units are in g-code,...
Internally software uses millimeters for all calculations and millimeters are used in settings file (which is not intended to be read/modified by humans anyway).

Settings attached are old. curacao now uses acceleration 2000mm/s^2 for motors. This is almost instant and it might even be too high for his mechanics.
Motion acceleration is even higher (5000mm/s^2). This means that machine will follow toolpath exactly and still have constant velocity.

With PlanetCNC TNG there is no need so slow on smaller arcs. We have feature called "Blend". It has tolerance setting and if distance from toolpath is greater than this tolerance then speed is reduced.
In other words - in constant velocity we do not allow deviance from toolpath to be greater than this tolerance. That is why our G64 constant velocity is not really constant if distance from toolpath is greater than set tolerance. We call this feature "blend mode".
So there is no need to slow down by 60% because TNG slows down if needed and still cuts at maximum possible speed.

I have no idea why his cut looks so rough. As I said, on our test machine with his setting and his g-code everything was smooth.

[robertspark]

Thanks for the insight + information

With regards to the slow down in feedrate to 60% it is a function requirement of plasma cutting not CNC motion.

The reason is angularity of the hole. If you cut holes at 100% linear feedrate you will find that the holes will be beveled internally.

The reason for this is because of the swirl of the plasma gas and also the trailing arc.

The discussion is detailed here (and many many other documents too):
Troubleshooting CNC plasma cutting: Part I - The Fabricator

[PlanetCNC]

Thanks for explanation. Plasma cutting is not my strong field. I'm more into milling.

[curacao]

Hello All,

Long story short. In my email conversation with PlanetCNC they hinted that the acceleration might be too high. I did some test cuts with a lower acceleration [of 500 instead of 1000] and the jaggedness of the cuts was reduced a lot. However the pausing of the torch at strange points during the cut is still there. I get the feeling the software is telling the controller to pause for a very small amount of time at certain points.

For now I am cutting again but still need to figure out this issue as it causes a lot of dross on the bottom of the cuts.


Here is a picture of the dross. Its not consistent everywhere because speed is not consistent. This is where it is the worst.


Atleast I am cutting now so I can fullfill my customer orders.

[robertspark]

I am happy to try to work with you to try to help figure out the issue if you want, but it will take some time to understand your setup, plus given I am not stood there a load of questions.

To start with
What is your current up to date settings, can you load a file I can trawl through though? Updated one of the previous file.


Can you explain your machine setup? By this I mean
Stepper motor amperage, torque, inductance rating (mH), resistance rating (ohms)
What stepper drives are you running, model
What power supply voltage are you feeding the drives
What micro step setting have you set on the drives
Is your machine direct drive or geared or has a belt reduction between the steppers and the drive?
What are you driving (belts, rack pinion, threaded rod, ballscrew, chain)
What is your pitch of your drive mechanism (1 turn of the stepper motor, how many turns of the drive mechanism or distance travelled (drive pitch)

The parts being cut, are they undersize? If so, by how much?

That should be enough at the moment to get a picture of your setup.

Rob

[tech-cnc]

hello sir
Any drawing program is used ?

[phamandp]

Hi guys, Could someone show me how to connect the hypertherm CNC cable to the MK3 please? Thanks a lot.

[PlanetCNC]

Do you meant the Plasma torch (ignition switch) connection?