Poor quality and Wavy Plasma cuts (Pictures)


Page 1 of 2 12 LastLast
Results 1 to 20 of 24

Thread: Poor quality and Wavy Plasma cuts (Pictures)

  1. #1
    Registered
    Join Date
    Jul 2006
    Location
    England
    Posts
    236
    Downloads
    0
    Uploads
    0

    Default Poor quality and Wavy Plasma cuts (Pictures)

    Hi
    I have had my homebuilt Plasma up and running for a few days now, and I am trying to get to grips with all the different cutting parameters.
    I have a Hypertherm 1000 with fresh Finecut consumables and it is using a Campbells THC300 Torch Height Controller.
    I definitely have clean air, because by luck I did manage to produce a good cut once......but in my excitement I did'nt note the settings....DOH!

    Two problems I am seeing a lot are 'Wavy' cuts and not great cut quality (See Pictures)
    The material is 16swg 304 Stainless Steel.
    I ran a load of test parts to find the best cutting parameters for the material as follows.

    Internal Holes
    40amp 47.25" (1200mm) per min at a cut height of 0.25mm

    Outside Profile
    40amp 138" (3500mm) per min at a cut height of 0.25mm

    I am using a homebuilt Water Table, and have the water about 1/2" below the surface of the material.

    Would cutting with Nitrogen improve the cut quality, and if so by how much?

    Any ideas would be much appreciated.

    Thanks

    Andy

    Similar Threads:
    Attached Thumbnails Attached Thumbnails Poor quality and Wavy Plasma cuts (Pictures)-plasma-1-jpg   Poor quality and Wavy Plasma cuts (Pictures)-plasma-2-jpg   Poor quality and Wavy Plasma cuts (Pictures)-plasma-3-jpg  


  2. #2
    Member
    Join Date
    Jul 2005
    Location
    USA
    Posts
    2415
    Downloads
    0
    Uploads
    0

    Default

    Those notches are not from using shop air. If the cut gap is staying constant with the THC the nodes are probably from a setting in MACH. Make sure you have the CV enabled and CV Feedrate turned OFF. Watch the torch. If you are seeing ragged movement and hesitation in the cuts then it's a software/setup issue. If tuned right and it should move smoothly through the cuts.

    Nothing like starting out on material that is a challenge to cut. Learning your machine by cutting mild steel is a lot cheaper and less frustrating way to optimize the cuts.

    Cutting at .25mm? The charts call for .063 inches for cut gap which is closer to 1.5mm.

    That's some pretty ugly cuts for a 40A tip.



  3. #3
    Registered
    Join Date
    Jul 2006
    Location
    England
    Posts
    236
    Downloads
    0
    Uploads
    0

    Default

    Thanks Torchhead
    Cutting at .25mm? The charts call for .063 inches for cut gap which is closer to 1.5mm.
    I am using Finecut consumables and the book lists 0.010" (0.254mm) for Stainless
    Nothing like starting out on material that is a challenge to cut. Learning your machine by cutting mild steel is a lot cheaper and less frustrating way to optimize the cuts.
    I did'nt think there was much use cutting mild Steel when I will be cutting Stainless Steel 99% of the time.
    I thought that if I got it cutting good on mild steel, I would then have to start all over again on the Stainless Steel???
    Make sure you have the CV enabled and CV Feedrate turned OFF
    I am using Mach3 Version 2.60
    CV mode is enabled, but CV feedrate was turned on.
    I also read last night that people who use the THC300 with thin material turn off the anti-dive for the THC.
    I will try all your suggestions.

    Thanks

    Andy



  4. #4
    Moderator
    Join Date
    Jan 2008
    Location
    USA
    Posts
    2247
    Downloads
    0
    Uploads
    0

    Default

    It looks like you have either a height issue or an issue with rough motion. Remember that the plasma torch is burning at a fixed power level....whenever the height control makes a correction....expect to see some sort of effect...usually a noticeable notch in the edge of the plate. For the same reason...if there is any roughness in motion...could be mechanical or part program or electronic.....then sudden changes in x and y velocity will create the same effect. If the velocity slows down...the plasma will just burn a wider kerf.

    First step in trouble shooting is to dry run through the part program...put your hand on the torch body....do you feel any roughness. If you can feel any roughness during motion...it will show in the cut. If it feels relatively smooth....then do this test again while cutting a part (plasma on, THC on)....if it now feels rougher than before...either quick z axis corrections or velocity changes/mechanical stiction....then you may have to adjust THC sensitivity or you may have issues with electrical noise interference that only ocurr with the plasma on.

    Jim Colt



  5. #5
    Registered
    Join Date
    Jul 2006
    Location
    England
    Posts
    236
    Downloads
    0
    Uploads
    0

    Default

    Thanks Jim
    I will try your suggestions.
    I tried doing a dry run yesterday and touching the torch. It seemed smooth enough to me.
    I will try again while it is cutting.

    Thanks for the input.

    Andy



  6. #6
    Registered
    Join Date
    Jul 2006
    Location
    England
    Posts
    236
    Downloads
    0
    Uploads
    0

    Default

    Well I tried the suggestions, and the cut quality has improved noticeably.
    The main culprit seems to be that the CV Acceleration was turned on (Thanks Torchhead )
    I still think that there is room for improvement.
    I think that the THC may need tuning because it seems to be going up and down many times a second to maintain a constant height (Approx. 5 adjustments a second)
    I will post a query on the THC300 forum to see what it should be doing

    Thanks

    Andy



  7. #7
    Moderator
    Join Date
    Jan 2008
    Location
    USA
    Posts
    2247
    Downloads
    0
    Uploads
    0

    Default

    In some cases you actually need to detune the THC. Either slow down the z-axis speed or deaden the response. If your machine had superior acceleration/deacceleration characteristics in the x and y directions (there are industrial machines that accelerate at 500 to 1000 mili gees) you can run the THC real hot....but if the THC has a faster feedback loop and faster response time as compared to x and y....it will cause a lot of quick voltage corrections that will show up as notches or pronounce arc lag lines on the cut face.

    Some THC systems have asynchronous control...meaning you can adjust the down corrections to be slower than the up corrections. If you think about it...this is a good feature as it minimizes unnecessary corrections that move the torch closer to the plate....while maintaining a very fast up speed to avoid collisions.

    Jim Colt



  8. #8
    Registered
    Join Date
    Jul 2006
    Location
    England
    Posts
    236
    Downloads
    0
    Uploads
    0

    Default

    Thanks Jim
    I think you are right about my THC
    I think it is why the cuts are 'wavy' because the THC is constantly adjusting itself up and down too fast????
    There is an adjustment on the Mach3 screen where I can change how sensitive the THC is, I just need to find out which way the adjustment works....

    I have read on the THC300 forum about manually setting up the THC first.
    You have to turn the THC off and set the material level so the torch can move along at a constant pierce height.
    You then do a test cut about 16"-20" long while watching the up & down LED's.
    You then adjust the course knob and find the 'Sweet spot' where the LED's are not flickering and the THC is not trying to move the Z axis.
    You then turn the THC on and note the position of the knob for future reference, and hopefully that will be that!..........fingers crossed.....
    I will try tomorrow and see what happens......

    Thanks

    Andy



  9. #9
    Member
    Join Date
    Jul 2005
    Location
    USA
    Posts
    2415
    Downloads
    0
    Uploads
    0

    Default

    Mach and the THC300 have a couple of parameters that will help tune the response. The THC300 is an analog control and the loop response time is partially determined by fixed components in the unit.

    You can tune the response of the actual THC by raising or lowering the THC Response number in MACH. That determines the reduced speed (percentage of max velocity of Z) that the Z moves will under THC control. A good number is 30%. It depends a lot on your Z speed. You want it set as high as you can (with a leadscrew) then tune the THC rate to make it cut evenly.

    The important thing it to watch the tip gap. If it's varying a lot then you need to do the tuning. Just because the Up and DOWN leds flash a lot does not mean the torch will move that often. Another thing to look at is noise. If plasma noise is getting into the tip volts signal back to the THC it will dance around a lot. If your table and plasma unit are not locally grounded (close rod in the earth) then disconnect the earth ground wire on the THC Sensor card. It may be injecting noise into the low side of the tip volts rather than draining it off.



  10. #10
    Registered
    Join Date
    Jul 2006
    Location
    England
    Posts
    236
    Downloads
    0
    Uploads
    0

    Default

    Thanks Torchhead
    My machine has stepper motors, and the Z axis uses a 3mm pitch screw.
    Its maximum speed is set to 960mm/min

    Andy



  11. #11
    Registered
    Join Date
    Dec 2004
    Location
    usa
    Posts
    28
    Downloads
    0
    Uploads
    0

    Cool Motion

    Just a small note to rule out any problems with motion make a small fixture with a pen that will slide up and down use a rubber band to apply pressure
    attach the fixture to the torch, Put a flat steel plate on the table with paper
    taped to the steel. And run a program to see what kind of motion you get
    I use this to test problems on my machines. Perfect lines= Perfect Parts.



  12. #12
    Moderator
    Join Date
    Jan 2008
    Location
    USA
    Posts
    2247
    Downloads
    0
    Uploads
    0

    Default

    Pen tracing is a good way to ensure that the machine has relatively fluid motion and is staying on path....but perfect pen tracings does not necessarily mean perfect cut parts. Here are a few things that will affect a plasma cut part on a cnc machine:

    1. Variations in speed/velocity. If the machine is continuously accelerating and de-accelerating...expect the cut edge to appear rough. Plasma requires a rather narrow (too slow/too fast) speed band for each material type and thickness and power level combination......and if the machine does not doo a good job of maintaining the speed even on intricate details....then the cut quality will defiinitely be affected. This is why more pricey cnc plasma machine manufacturers go to great pains to have very high acceleration/de-acceleration capabilities. When the plasma is operated at slower cut speeds...the kerf naturally gets wider...changing part dimensions.

    2. Torch height control. If the torch height control system does not accurately maintain torch to work distance within about .005" of the correct height....the the cut edge will be affected in terms of angularity and kerf width. Also...if the THC is overcorrecting...best described as a "sewing machine motion", expect very pronounced lag lines on the cut edge.

    3. Occasionally we see issues where with a pen tracing we see very smooth contours...but when the plasma torch is active....the cut edge is very rough. Often the rough edge is dismissed as "that's the way plasma cuts". In reality....roughness during the cut could be an effect of electrical noise interference that is generated by the plasma power supply (many are inverters operating in the 20 khz range) capacitively or inductively coupling to the feedback loop for the servo drives (or stepper drives)....which can cause anomolies with the motion...usually shows up as a rough cut edge. This can usually be felt by resting your hand on the torch body while cutting...if there is any vibration during motion...expect to see it in the cut face.

    Jim Colt



  13. #13
    Registered
    Join Date
    Jul 2006
    Location
    England
    Posts
    236
    Downloads
    0
    Uploads
    0

    Default

    Since my last post, I have been trying a few things.
    Each one in turn has improved the cut quality

    I had a problem with the THC300 causing the Z motor to oscillate.
    I placed a small piece ot sticky tape on the Z motor shaft, and I could see how the Z motor was reacting to the THC
    Mine was oscillating about 1/4 of a revolution (45°) about 4 times a second.
    My Z axis has a 3mm pitch screw, so that worked out that the torch was going up and down approx. .4mm (0.015")
    I had to turn the THC rate down to 10% to stop the oscillations.
    I calculated that at this Z Speed, the sheet can warp by 50mm high over the length of my bed and the THC will still cope

    After a lot of experimentation I managed to understand the workings of the THC
    I found the best method was to do a manual cut, with THC and anti-dive turned off.
    I write a program to cut a line approx. 500mm long at the cut height specified in the Hypertherm manual.
    I then watch the Tip voltage and note the voltage.
    I then do the same cut with the THC turned on, and anti-dive turned on.
    I then turn the THC course knob to match the previous voltage.
    This method produces a perfect cut

    After all this I was still getting problems on more intricate cutting.
    I was told to turn off all the CV settings, but to leave CV Mode turned on.

    All these mods and it is now cutting O.K
    I have noticed that sometimes even when cutting identical pats, you get differences of cut between the parts. So it always best to run several parts and take an 'average' to judge the cut quality.

    Thanks for all your input everyone

    Andy



  14. #14
    Registered
    Join Date
    Jul 2006
    Location
    England
    Posts
    236
    Downloads
    0
    Uploads
    0

    Default

    Just a small note to rule out any problems with motion make a small fixture with a pen that will slide up and down use a rubber band to apply pressure
    attach the fixture to the torch, Put a flat steel plate on the table with paper
    taped to the steel. And run a program to see what kind of motion you get
    I use this to test problems on my machines. Perfect lines= Perfect Parts.
    I have still not been 100% happy with the cut quality and I have been using the pen method to take the Plasma and THC out of the equation.
    Using the Pen method I still get wavy lines, so it boils down to 2 things, a CV setup Problem or a mechanical error.
    It draws holes (circles) perfectly but it draws wavy when cutting lines and arcs like slots etc.
    I 'drawn' a shape that I had cut out previously with the plasma which had wavy cutouts, and the drawn part matched it and it was just as wavy......
    I have CV Mode enabled and CV Feedrate turned off.
    I am thinking that it is a CV fault more than a mechanical problem.
    My machine is dual purpose and when it is a router it cuts perfectly.

    Any ideas would be appreciated.

    Andy

    Last edited by Normsthename; 02-26-2008 at 03:18 PM.


  15. #15
    Registered
    Join Date
    Jul 2006
    Location
    England
    Posts
    236
    Downloads
    0
    Uploads
    0

    Default

    I have CV Mode enabled and CV Feedrate turned off.
    I am thinking that it is a CV fault more than a mechanical problem.
    I have been doing some more testing with the pen tracing.
    The result was very jerky and wavy tracings
    I have narrowed the problem down to the radiused corners.
    When drawing these it was very jagged, you could'nt even recognise the shape!
    I tried lots of CV settings and eventually ended up with a reasonable trace.
    I then tried slowing the acceleration of the X & Y Motor from 600 down to 300 and there was a noticeable improvement, not perfect but close.
    I then slowed the acelleration down further to 200 and the tracing was perfect
    But I am back to an old fault where the machine pauses for a split second on every start and end of a radius.
    Anyone know how to fix this?
    Would drawing the arc as a segmented polyline / polygon instead of an Arc make any difference??
    I will give it a try tomorrow....

    Thanks

    Andy



  16. #16
    Registered
    Join Date
    Feb 2008
    Location
    Canada
    Posts
    121
    Downloads
    0
    Uploads
    0

    Smile

    Would like to see some pics of your cuts now that you got things almost figured out!



  17. #17
    Registered
    Join Date
    Jul 2006
    Location
    England
    Posts
    236
    Downloads
    0
    Uploads
    0

    Default

    Since my previous post I have managed to cure the 'Pausing' problem.
    Everyone says to have CV Mode turned on, and everything else relating to CV turned off.
    The problem (for me) was that with just CV on and everything off the machine rounds all sharp corners quite a lot.
    I found the optimum settings for me were the following :-

    CV Mode ON
    All CV Related items turned off EXCEPT for CV Dist Tolerance which is set to the default 0.9
    This along with slowing the acelleration down to 200 has made my machine do perfect Pen Traces

    Would like to see some pics of your cuts now that you got things almost figured out!
    I will post some sample cuts very soon!

    Andy



  18. #18
    Member
    Join Date
    Jul 2005
    Location
    USA
    Posts
    2415
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by Normsthename View Post
    Since my previous post I have managed to cure the 'Pausing' problem.
    Everyone says to have CV Mode turned on, and everything else relating to CV turned off.
    The problem (for me) was that with just CV on and everything off the machine rounds all sharp corners quite a lot.
    I found the optimum settings for me were the following :-

    CV Mode ON
    All CV Related items turned off EXCEPT for CV Dist Tolerance which is set to the default 0.9
    This along with slowing the acelleration down to 200 has made my machine do perfect Pen Traces


    I will post some sample cuts very soon!

    Andy
    HOLY S*** Andy: 200 for accel? That means you are accelerating at 12,000 IPM/sec. If your feedrate is say 200 IPM you go from 0 to full speed in 16 milliseconds! Try that in your car (:-) In MACH accel is in IPS/s rather than IPM units (like velocity) which makes it 60 times faster. I would think a number like 20 to 30 would be closer to optimum.



  19. #19
    Registered
    Join Date
    Jul 2006
    Location
    England
    Posts
    236
    Downloads
    0
    Uploads
    0

    Default

    HOLY S*** Andy: 200 for accel? That means you are accelerating at 12,000 IPM/sec. If your feedrate is say 200 IPM you go from 0 to full speed in 16 milliseconds! Try that in your car (:-) In MACH accel is in IPS/s rather than IPM units (like velocity) which makes it 60 times faster. I would think a number like 20 to 30 would be closer to optimum.
    I am one of those funny people that uses metric
    200 works out to just under 8"
    I initially had it set at 600 (23.62") which is in between your optimum settings.
    But my machine is made from steel tubing and the Gantry is made from 1" Steel Tubing which makes it quite heavy.
    It was originally made that strong for Routing.
    Now I mainly use it for Plasma I wish that I had made the Gantry much more lightweight
    Hindsight is a lovely thing.....
    When funds allow I would like to upgrade the machine to linear bearings throughout and also make a new lightweight gantry.
    I could then speed up the acelleration and get better cut quality.

    Thanks

    Andy



  20. #20
    Registered
    Join Date
    Feb 2006
    Location
    uk
    Posts
    24
    Downloads
    0
    Uploads
    0

    Default an issue os stainless

    i have cut stainless recently and after much cutting of normal steel am frustrated by the quality of stainless cut. is it customary to have black jagged finish?



Page 1 of 2 12 LastLast

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •  


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

Poor quality and Wavy Plasma cuts (Pictures)

Poor quality and Wavy Plasma cuts (Pictures)