Need Diagnosis of my cut problems (new machine)

[DesertFabworks]

I have my new machine up and running and have been doing some test cuts. I have found a few problems
and would appreciate some help troubleshooting them.

System: iplasma 4x8 table, powermax 65, dragon cut system, sheetcam, mach3

The tests pieces in the picture were cut in 16g steel using fine cut consumables
45 amps.

Picture one is exactly per the hypertherm specs. There is no dross
Picture two is same setup slowed from 250 ipm to 200 ipm now I have dross very little improvement on holes or wavy lines
picture three is slowed to 150 ipm lots of dross very little improvement on wavy ness.
picture 4and5 are of the wavy cut lines

Problem #1: wavy cut path in circles and around the corners good and straight on straight aways

Problem #2: Parts are not square. if I tell it 3" wide its 3" wide on the dot but part is not square see pic

Problem #3: Circles are not as round as I would like most likely related to problem one and two.

Cut is pretty square not machinest square but good I believe for plasma.

Any help is appreciated!!!!

[Gamelord]

I am not sure on the other issues, but the wavy lines I know very well. I had this problem with my table and there are two things that will cause this.

1) Slat movement. If your slats in your table are moving, as your gantry moves from one direction to the other, it will "shake" your table, making your slats move or "wave" back and forth very slightly, giving you the wavy lines around the corners. To check for this, check your slats and see if they are solid. I found that when doing small scrap pieces of steel, I need to lay out other pieces of steel on my table around the areas to "tie" the slats together and minimize slat movement. When I change my slats out of my table this next time, I am going to put them into a wave shape instead of just straight across the tale like they are now. This should put the slats into a bind which should eliminate any slat wave. This would be why the wave would be a little less if you slow the cut speed down, the change in direction is much less abrupt, giving less slat wave.

2) If your slats are solid, then it is most likely your gantry shaking as it changes direction. (I had both of these issues on my table). To fix this, you need to make sure your gantry is rock solid and can't wiggle or shake as it changes directions. This could be caused by warn bushings, loose gears, poor adjustments, etc... Even the slightest amount of movement (1/32") will give you the wiggle lines that you are seeing. This is why it is only showing up on the corners, when the gantry changes direction, it wiggles a little until it settles down and finishes the cut, then when it changes direction again, it wiggles again. If you only see the wavy cut on two of the sides, then you can narrow down if it is forward /backwards or left/right movement. For my table, if it is waving on the top and bottom, it would be movement in the X axis. If it has waves on the left/right, it would be movement in the Y axis. If it is moving on all four sides.....well, you got something very loose all over.

As for the square cut issues: This is an issue with either your software, settings, motor issues or your table is not square. Again, check to make sure your motor's are not moving/walking and are locked in place. Any odd drifting on your motors will cause this. Because all the pieces appear to be out of square the same, I would say it is more likely that your table is out of square or your software/settings are faulty.

Others may have more data for you....hope this gets you going in the right direction.

[DesertFabworks]

I believe that like you said it is in part due to gantry wiggle. I tightened everything up and saw a definite improvement.

I believe that some of the wiggle is due to the design of the system and I dont think that I can eliminate all of it especially at the higher speeds of 250+. I cut some 1/8 plate and saw no signs of the wiggle at 95 ipm.

I thought that my system was out of square also but checked and re-checked. I saw some improvement with taking the wiggle out of the gantry. I will pursue this more and see if it helps.

Thanks for the ideas, It helps to have some fresh ideas.

[Oldsarge]

Also, check your motor tuning page in Mach, if you are using a slaved axis on the Y your slave (A?) should have the same exact step numbers.... Put a sheet on your table and line it up off the side rail, then center your torch over thedge, and run the gantry along the edge of the plate... should run true the entire length of the sheet.. if not then there's a squareness issue with the gantry.... Also, check check check that your pinion gears are tight.... a slipping gear will have you chasing a good cut... ask me how I know! If your set screws are questionable like mine were, I pulled them and replaced with socket head set screws and used lock tite and a whole bunch of my cut quality issues went away...

Good luck, hope some of this helps. It's awesome when a build comes together!


Oldsarge

[I Lean]

In addition to the other stuff that has been mentioned, lowering your acceleration numbers can help with the wiggle. What is your accel set at now?

[DesertFabworks]

Thanks for all the info.

Found some slip in my pinion gears, added some locktite and a little torque

My acceleration is set at 35 which is what the manufacture recommended

My settings in mach are the same for slave axis so that is good.

With these fixes It is mostly gone, I'm square so that it good. Still having trouble dialing in the
perfect holes. I may be asking too much. Not sure how small I can go with this setup and get
decent holes. Its not a high def plasma, but I was wanted to get nice 1/4 inch holes.

[Gamelord]

For the holes, are you piercing away from the edge? It looks like you are piercing right on the edge which is giving a bump-out. If you have the ability to do so, create a lead-in so that your pierce is away from the edge and the torch leads into the hole to create the circle. The same will need to be done with the lead-out so the torch moves away from the edge when it finishes. That combination along with removing the "wiggle" should get you some pretty good holes.

If the holes need to be perfect, what I will usually do is to make the hole .10 under with the torch, then drill them out with my press to the exact size required. This makes drilling super easy. If you are doing a zillion holes, this would be a pain though.

[DesertFabworks]

I was using a .25 lead in arc and .25 lead out arc to do the holes. I have done the step drill trick for holes in the past. The come out looking great but I would like to have the plasma machine make them great in one shot. I think I need to just keep tweaking.

[Oldsarge]

If you have a. 25 lead in on a. 25 hole you may be getting too close on both lead in and out lead out. I usually do. 17 and get decent holes. Also, if you did find some play in your pinions then you need to redo your steps per inch so they are as accurate as possible. I played with mine till I was within. 0004 on my x and dead on on the y and my oblong holes were round! Stick with it, you'll have it dialed in in no time!

Oldsarge

[jimcolt]

For best quality on holes:

-Use a lead in that gets as close as possible to the center of the hole for 2 reasons: 1. There usually is a slag puddle on the top of the plate..if this puddle stays on the radius (contour) of the hole, it will cause the plasma arc to waver and create a divot or ding in the hole. 2. A longer lead in gives the plasma arc time to stabilize (pressure and energy take a while to ramp up), also allows the height control to index down to cut height before it gets to the contour of the hole.

-With an air plasma, it is best to have no lead out. Let the arc shut off right at the 360 degree position on the hole contour. Some software has provisions to keep the arc on for a time period after the motion stops....on steel under 1/2" this usually is not necessary.

- Cut speed on holes should be right at about 60% of the speed used to cut the outside contour of your parts....this will create some low speed dross on the bottom of the hole, but will minimize taper in the hole. Some machines will do this automatically on all holes under a certain diameter, such as 1", while other software may have to have the G Code manipulated to achieve this.

-Ensure that cut height is correct. Usually on holes under 1" diameter it is best to disable arc voltage control....allow the pierce height, allow indexing to cut height, but don't allow arc voltage height correction...as the slower speed used for cutting holes will cause the arc voltage height control to move the torch too close to the plate.

-Try spraying some mig welding anti-spatter spray on the top of the plate before cutting. You may be surprised at the improvement in hole quality. The spray usually makes the top spatter from piercing non -existent,minimizing arc wobble on holes. While you are at it spray a little on the front of the torch to keep spatter off the shield/nozzle. Do not use the dip type, and I recommend the water based spray vs silicone or oil based.

-last, but not least....use the lowest powered consumable set recomended for your material thickness for best hole quality. This will reduce cut speeds but will give you better results. If it is Hypertherm use FineCut consumables for all holes on material thicknesses under 3/16", 40 Amp shielded consumables for thicknesses above 3/16" to 3/8", 60 Amp consumables for thicknesses above 3/8" to 5/8".

The nozzle and shield orifices must be perfectly round, no nicks, dings or craters. Inspect with a 10x eye loupe....if they are not perfect, use these parts for hand cutting or contour cuts that are not as critical. The orifice shapes the arc, the arc shapes the part you are cutting. Piercing too close or too thick can damage a nozzle orifice in one pierce.

Bottom line on hole quality.....use the right speed, the best power level, height control, height control, height control.

Jim Colt

[benval76]

Are the same parameters recommended for small diameter circles as well? I ask this because I have been having some cut quality issues recently cutting some 2 and 3 inch discs for pipe caps. At what point would it be recommended to run with the height control off and reduced speed? I am running a HPM 85 with Torchmate Cad.

[jimcolt]

It will be the same....holes and circles under about 1" should be cut without arc voltage control active....and it is a good rule to run at 60% of the suggested cut speed.

Jim

Are the same parameters recommended for small diameter circles as well? I ask this because I have been having some cut quality issues recently cutting some 2 and 3 inch discs for pipe caps. At what point would it be recommended to run with the height control off and reduced speed? I am running a HPM 85 with Torchmate Cad.