Masso pauses during plasma cutting and routing. (PAUSE PROBLEM HAS BEEN FIXED NOW. WITH A BUG FIX)

[Ross]

It looks like we are having problems in trying to eliminate the pausing motion while running G-code when doing a job.

Here is my statement from the other post!

From Ross.

Came from - (Plunge rate sheet cam) post.

------------------------------------------------------------------------------

Reig and cncburn, I have the same problem with the Masso pausing on movements,

Mach3 post is no good cause it won't convert to curves!

The thing that i have noticed with the Masso post is the pause is at the moment it is getting the command to do an ark and at the same time the Masso run light that i added blacks out for a split second. probably in the lines that i have high lighted red.

If you watch the jeep i cut you really see it while cutting the wheels and the feed will drop to 0% "might be processor speed or a bug not sure, but i sway towards processor speed"

From Ross.

N0340 X59.5743 Y38.6227
N0350 X59.5981 Y38.6329
N0360 G03 X60.7326 Y39.1852 I-3.3724 J8.3690
N0370 X61.3080 Y39.6117 I-1.6023 J2.7631
N0380 M666 (---THC Off---)
N0390 X61.1631 Y41.4857 I-0.9430 J0.8697 F3060.0
N0400 G01 X61.0884 Y41.5576 F3400.0
N0410 X60.2234 Y42.5633
N0420 X60.2055 Y42.5852
N0430 X59.8743 Y43.0130
N0440 X59.3023 Y43.7186
N0450 M667 F130 (---THC On---)
N0460 G02 X58.4933 Y44.7986 I7.1929 J6.2314
N0470 X58.9092 Y51.7393 I4.1446 J3.2345
N0480 G01 X59.5579 Y52.5000
N0490 X59.5816 Y52.5354

Jatindar if you want the JEEP cut file call me on Skype and i can send it to you!

 

[masso-support]

Hi Ross

I was going to give your Gcode a try on my machine but mine isn't big enough unfortunately.

Is Sheetcam able to do a convert the drawing to circular ars before you run the post processor on it? That's what I do in Vectric software to get smooth motion.

Cheers

Peter

 

[breezy]

@ross, @masso-support

Have attached videos of the Bicton Men's Shed router in operation cutting circles, showing the pause between each quadrant. The code is ramping at 10deg to full depth of the material and you can see the stops/pauses in all axis at each quadrant.

This is a portion of the code that was running

(BOTTLE)
N30 M5
N35 T5 M6
N40 S20000 M3
N45 G54
N50 G0 X232.047 Y225.896
N55 G43 Z31. H0
N60 Z21.
N65 G1 Z18.5 F5000.
N70 G3 X167.953 Y274.104 Z14.101 I-32.047 J24.104
N75 X232.047 Y225.896 Z9.702 I32.047 J-24.104
N80 X167.953 Y274.104 Z5.302 I-32.047 J24.104
N85 X232.047 Y225.896 Z0.903 I32.047 J-24.104
N90 X240.1 Y250. Z0. I-32.047 J24.104
N95 X159.9 I-40.1 J0. F10000.
N100 X240.1 I40.1 J0.
N105 G0 Z31.

Regards,

Arie.

 

[masso-support]

Interesting Arie

I just run your file on my machine and it runs smooth.

I removed the M6 for the video but it runs the same with it as it does without.

 

[testyourdesign]

Hi Peter,

Just a thought. Are you guys using backlash compensation? I noticed a slight pause on my machine after adding a value to backlash compensation.

Cheers, Stephen Brown

 

[breezy]

Quote from testyourdesign on October 28, 2019, 10:58 am

Just a thought. Are you guys using backlash compensation? I noticed a slight pause on my machine after adding a value to backlash compensation.

I do have backlash turned on. Because our machine uses belt drives and can't remove all the backlash by tensioning the belts.

Have attached the full file (Zip). There are six pieces cut from a 1200 x 800 sheet of ply. The first file pre-drills holes for hold down screws, second cuts to 2mm from the bottom and rounds-over the edges and the third after flipping the sheet over and probing the centre of the far right bottle hole, drills holes for hinges, rounds-over the handle & bottle holes, finally completing the cutout & round-over.

Regards,

Arie.

 

[Ross]

Quote from MASSO Support on October 28, 2019, 9:39 am

Hi Ross

I was going to give your Gcode a try on my machine but mine isn't big enough unfortunately.

Is Sheetcam able to do a convert the drawing to circular ars before you run the post processor on it? That's what I do in Vectric software to get smooth motion.

Cheers

Peter

The Masso post script has the convert to arcs built into it, so all the magic is done in SheetCam from that.

So all you do is load a DXF, pick the tool and press the P (Run the post processor.)

The post processor that i use, i modified and has a scribe code added to it.

Masso post script pauses as well if loaded in SheetCam.

You might be able to try this tap file.

From Ross.

 

[Ross]

Not using backlash on mine!

From Ross.

 

[masso-support]

Hi Guys

I reran the file with Backlash enabled as suggested by Stephen and now have motion as shown in Arie's video and as described by Stephen. Whenever backlash compensation is enacted I am seeing a pause as the axis reverses direction to take up the backlash. Not much you can do about backlash with a belt drive Arie.

I looked at the Butterfly and the Gcode looks ok and there is what looks like the right mixture of arcs and straight lines for the piece being cut. I tried to run it but the Z axis probes every cutout and it does not appreciate plunging onto the touchoff block at those feedrates. My spindle doesn't quite float like a plasma torch. I will have to go through and manually modify the code to run it.

That said The Post Processor does not convert the drawing to arcs. That is the job of Sheetcam itself. The Post processor simply formats the Gcode so if there is a circular arc in the drawing it will output an arc in Gcode. Lines and Bezier curves output as a series of straight lines. I got caught recently thinking that a bezier curve was an arc and I couldn't figure out why it was output as lines in Gcode until I realized that Gcode only describes circular arcs and not random curves. Didn't I feel foolish. They may look the same in a drawing but they are nothing alike.

Masso runs exact stop machining and not Constant velocity. Exact stop is more accurate and Constant velocity is the same as saying 'I would like you to cut something that looks a bit like this".

Constant velocity smooths out the motion and keeps speed up by literally cutting corners. It converts lines to arcs on the fly and making 2 pieces fit together that have been cut using constant velocity can be a challenge. If you want to smooth the motion out you are better off converting it in your CAD software where you have control of the final shape of the piece as the PC processor is far more powerful and can take it's time working it out.

In Sheetcam it looks like the conversion to Arcs is automatic and determined by the Arc Fitting Tolerance setting in the drawing input tab.

Cheers

Peter

 

[breezy]

Quote from MASSO Support on October 29, 2019, 8:35 am

I reran the file with Backlash enabled as suggested by Stephen and now have motion as shown in Arie's video and as described by Stephen. Whenever backlash compensation is enacted I am seeing a pause as the axis reverses direction to take up the backlash. Not much you can do about backlash with a belt drive Arie.

OK. I'm happy with that. I prefer true shape to distortion caused by backlash.

Quote from MASSO Support on October 29, 2019, 8:35 am

The Post processor simply formats the Gcode so if there is a circular arc in the drawing it will output an arc in Gcode. Lines and Bezier curves output as a series of straight lines. I got caught recently thinking that a bezier curve was an arc and I couldn't figure out why it was output as lines in Gcode until I realized that Gcode only describes circular arcs and not random curves. Didn't I feel foolish. They may look the same in a drawing but they are nothing alike.

That would explain the lumpy finish that I had on the Christmas Cars project. I had drawn them in Fusion using splines which is their term for Bezier curves. I reduced the number of code lines by upping the "Smoothing & Tolerance" settings, but there are lots of arcs and lines interspersed. As per sample. The whole file was 7615 lines of code to cut out six cars about 140mm long, this was roughing & finishing cutting.

N5900 G2 X144.442 Y58.971 I-0.768 J-4.941
N5905 G1 X147.316 Y58.282
N5910 G2 X147.655 Y58.188 I-1.166 J-4.862
N5915 G1 X150.352 Y57.337
N5920 G2 X150.64 Y57.236 I-1.505 J-4.768
N5925 G1 X153.112 Y56.287
N5930 G2 X153.361 Y56.183 I-1.793 J-4.668
N5935 G1 X154.158 Y55.843
N5940 X154.95 Y55.489
N5945 X155.734 Y55.12
N5950 X156.512 Y54.738
N5955 X157.284 Y54.342
N5960 X158.048 Y53.932
N5965 X158.804 Y53.509
N5970 X159.553 Y53.073
N5975 G2 X159.771 Y52.942 I-2.474 J-4.345
N5980 G1 X161.156 Y52.057
N5985 G2 X161.376 Y51.908 I-2.692 J-4.214
N5990 G1 X162.576 Y51.048
N5995 G2 X162.777 Y50.896 I-2.912 J-4.065
N6000 G1 X163.441 Y50.24

Regards,

Arie.

 

[Ross]

Peter, I had a brain storm of an idea to test plasma files.

Pull a spring out from a ball pen and stretch a bit longer, place into the chuck that will give a bit on touch down.

Place a flat piece of metal on the table to finish the circuit, Eg: the wife's aluminium oven pan might do.

Just keep it simple. OH don't forget to have the spindle turned off!

From Ross.

 

[masso-support]

Hi @ross

Thanks for the Butterfly file.

I ran it on the mill and it ran exactly as expected so I loaded the Plasma software and gave it a try.

Much to my surprise it stuttered it's way around the table. I went back and started removing Gcode commands from the file until it ran smoothly and i found that removing the THC instructions on and off allowed the motion to return to proper motion.

I then noticed that the THC indication was turning on and off like some sort of Christmas tree light.
N0180 M03 (---Torch On---)

N0190 G04 P300.0

N0200 (---Go to cutting height---)

N0210 Z1.5000

N0220 G01 F1000.0

N0230 G03 X28.1825 Y23.0930 I-0.1668 J-2.5546 F3060.0

N0240 G01 X28.1347 Y22.3612 F3400.0

N0250 G03 X28.7020 Y21.6543 I0.6844 J-0.0318 F3060.0

N0260 G01 X28.7957 Y21.6294 F3400.0

N0270 M667 F130 (---THC On---)

N0280 G03 X39.2993 Y22.9258 I3.9796 J10.9558

N0290 G01 X39.3140 Y22.9411

N0300 X39.3634 Y22.9868

N0310 M666 (---THC Off---)

N0320 G03 X39.9594 Y24.9610 I-1.1665 J1.4292 F3060.0

N0330 M667 F130 (---THC On---)

N0340 X38.5868 Y26.1863 I-2.0526 J-0.9179 F3400.0

N0350 G01 X38.5258 Y26.2098

N0360 G03 X31.3690 Y26.6116 I-4.0962 J-9.0219

N0370 G01 X30.5614 Y26.3551

N0380 X30.4973 Y26.3389

N0390 M666 (---THC Off---)

N0400 G03 X28.1801 Y23.1915 I0.5346 J-2.8203 F3060.0

N0410 M05 (---Torch Off---)

You can see in the Gcode above that the THC turns on and off twice in the process of cutting the first small hole in the butterflies wing. This is the reason for the hesitations that you are seeing when it runs the Gcode file.

I would have thought that after turning on the Torch you would turn on the THC and it would remain on until you turned off the torch.

Instead the THC is being turned on and off randomly throughout the cut which results in the hesitant motion. It doesn't turn on until partway through the cut.

I think if you modify the Post Processor to add THC on immediately after moving to cutting height and off before the M05 it will sort out your motion.

Cheers

Peter

 

[Ross]

Peter do you think this is all i need to remove from the post processor. hi-lighted in pink

or is it best to hand my post script to Masso to fix.

Remember mine has the scribe added to it!

from Ross.

(The turn off THC is to stop the torch crashing when it slows down on curves) If really needed not sure cause the time that is off isn't very long!

 

[masso-support]

@ross

I'm thinking now that your GCode is correct Ross.

I had a chat with Jat this evening and he mentioned the same thing that you did in that the axis needs to be turned off when the speed drops or the z axis will crash. That explains the THC turning on and off throughout the cut. Probably better off not touching the Post Processor. I learn something new everyday and what sounds logical to me isn't always the case. (I really need a plasma)

It seems when it reaches a THC on / off it stops the motion and then has to restart moving again once the THC is sorted causing the hesitation.

I don't have an answer for you at this time and will need to do more testing to get a better understanding.

Cheers

Peter

 

[Ross]

Hi Peter and Jat, I sent my post script to Masso support vi-are Skype for you both to look at, That I painstaking made.

It also has the Scriber M-codes and off sets added to it which is working!

From Ross.

 

[masso-support]

Hi Ross,

Sorry for the delay in getting back to you. I haven't seen your Post processor unfortunately as I don't have access to the Skype account but I have been doing some testings to get a better understanding of how Masso treats the THC on / off instructions. I now know that when Masso reaches the THC code it stops , executes the instruction and then starts moving again. This is the pauses that you and I are seeing in the GCode and is the way Masso works at present.

The next part to understand is why there are so many THC on / off commands in the Gcode. If I understand correctly from what you have said, when the plasma slows down for corners the torch has a tendency to drop and crash so the THC is turned off and switched back on once the torch is up to speed again. This means you cannot turn the THC on at the start of each toolpath and off at the end as I had originally thought.

Looking at the Proma manual there isn't much in the way of adjustment. Would changing the Hysteresis or Time delay will not help with the cornering issue or would this cause other problems?

I would be interested on knowing yours and others thoughts on this as the finer points of plasma machining are new to me. I'm sure there are gaps in my knowledge, is there anything I have missed?

At this stage I'm just trying to get a fuller understanding of how things work in the Plasma world and then go from there.

If you want to send your Post Processor could you open a ticket and post it there and that way I will be able to see it.

Cheers

Peter

 

[ae_mike]

I agree with Ross, sure would be nice if the path didn't stop/pause for a THC on or off command. I've tried small radius corners with and without with mixed results. Sometimes with it on, things go crazy with my Proma height control even with the Z speed turned down and with THC off and the pause/delay, I get more dross (those ugly hanging bits of slag/metal) than I want. I'm about to try to just to chamfer the corners and leave the THC on and see what happens. I'm just so used to putting radii on my corners to make things pretty and safe that chamfers are going to be struggle to remember.

BTW, I'm about to post my corrected post processor for SheetCam. Found and fixed a few more things as I burn more parts. Main difference is the addition of the drill functionality which is really important for my work but some other fine tuning options.

Regards,

Michael

 

[masso-support]

Thanks @ae_mike

That's the sort of thing I'm looking for to get a better understanding of Plasma. I know that arcs are the best way of doing a corner on a mill so that you don't need to stop.

Could I just show my ignorance and ask what a chamfered corner looks like?

To me a chamfer is a bevel on the edge of something so I'm not sure what it would be on a plasma machine.

Cheers

Peter

 

[ae_mike]

Hey Peter,

You have it right, a chamfer is just a straight line that connects 2 other edges. Typically at a 45 degree angle. You are thinking of them on the front or the back surface but they could be better any 2 surfaces just like a radius. common in CAD to either radius/blend an edge or to chamfer it. In my case with 12 gage steel, I'm either putting blends on 0.105" long edges or I'm putting chamfers on those same short edges. My thought is since a chamfer is just another straight line and not a radius, the post processor would see it as a G01 command and not as a G02 or G03 and then wouldn't turn the THC off. I'm kind of tempted to try the G02/G03 without turning THC off again now that I have things tuned better just to see if anything bad happens. Guess I'll run a test part and see what happens.

Regards,

Michael

 

[jim-in-michigan]

@ross

I looked at post 3967 and did not see any physical evidence of any damage.

Thanks for the help

Jim