Warpage, and I'm not talking Star Trek..

[MountainWerks]

Hi Guys.I discovered CNC plasma about a year ago and got hooked. I’m lucky enough to have a local community college that has a machine in a makerspace they have on campus which has allowed me to begin to learn the basics at night and on the weekends. I’m cutting my teeth on that before buy my own and and am in the process of getting electrical done in my garage in preparation. I’m going to be doing mostly art and possibly some welding tabs/industrial parts. I have been having some trouble with some designs that I was hoping the brain-trust here might help with regarding warpage. Before I begin I have done a search for “warpage” and read was was posted there which gave me some good ideas already but I still need some help.

The machine I’m working on is a CanaCNC from what they tell me (I think) and it’s not really set up ideally from the limited information I have. It’s at a community college so it’s kind of beaten on so not dissing the company. There are issues with the torch height control which is not working and it has a “click” type physical height switch that doesn’t seem to be calculating the cut height. This means we have to estimate the length of nozzle contact to material and the audible “click” when the switch triggers and plug that into Sheetcam and add in ideal torch cutting height to get the proper total cutting height. The frame is also not solidly welded together and when running 240ipm the whole table jiggles slightly which I would imagine leads to wobbly cuts which I’m experiencing. I’m trying to do some trouble shooting for them. Here is the setup as best I know.

Powermax 45 running standard consumables using several loops of pipe as a water trap. No filter that I see, but haven’t looked closely.
Kerf width set to .053
Feed rate 240 per manual they gave me (but not sure it’s the right Powermax manual. I downloaded another one that said 350-400?). I think the table maxes in the software at 240ipm
Pierce delay .1
Plunge rate 3.937
Water table about half full. I’m just cutting 16 gauge. Cold rolled shows much less warpage than hot rolled. Water does splash on the sheet during cutting (I read you don’t want water in the table to prevent warpage?)
Software: Adobe illustrator>Sheetcam>Mach3

Pictures of the table





Here is a project I did for my daughter out of 16 gauge cold rolled. Space between the words is about and inch or two, bridges between letters to hold the inner part of e,o,a, is about an eighth. The piece is about 23.5x20 and only has very subtle warpage and it lays flat when mounted on the wall.



This is a similar project I did out of hot rolled that I’m having bad warpage on as you can see. (They were not rusty when I cut them, they’ve been out in the rain). It’s much tighter than my daughters sign in terms of distance between the words (about a half inch between words and bridges are about an eighth like the other one). As you can see some of the lines are not very straight. Does that look like a normal amount of dross from you guys who have systems dialed in? The dross can be hard to get off. I’m getting 75% of the way through cut-outs as intricate as this, and then getting nozzle-dragging the warpage is so bad.








Couple questions I have:
What can I do to mitigate the warping? Set-up, material, cut paths?
What setting on the machine should I play with?
Since I’m new to plasma cutting, am I asking for too much detail in my graphics files? (or maybe I’m just asking too much details for THIS CNC system as it’s set-up).

Thanks Guys!

[djreiswig]

That's a lot to digest.
The switch should be fine. I'm assuming you are running Mach3. There is a setting in Mach 3 as well as in the SheetCam postprocessor where you put an offset distance for the switch. If you download the CandCNC manual for your controller model it should walk you through how to determine this figure.

I try to run my water bed level as high as possible to help with warpage. You can change the path order in SheetCam to a setting that will move around the part more instead of cutting everything in one area all at once.

Cut height is very important. If your initial setting is off, it only goes downhill from there. I think if you can get the torch height control working you will have much better results.

Using fine cut consumables also helps.

If you can get more information on which controller and what torch height is on there it will help with troubleshooting.

[ben de lappe]

Hi MountainWerks! Welcome to the site. Granted, cad is my area but here's my take.
Pretty well every topic you discussed will influence warpage. From cut height, amps, speed of travel to amount of material removed from what area and how much support is in the surrounding piece. Perfect example, the above pic showing warpage with the lettering cut out of the middle of the 16ga. plate. Your torch spent a lot of time in that area putting out a lot of heat but there are ways to combat that. Don't try to cut as fast as possible. I never ran top speed specs. Even with a "tight" machine. What I did do was find a proper amperage to set my plasma and the proper travel speed to give me the desired cut. I loved my 12ga. cold rolled, still remember my setup. 45 amps and 145 ipm., cleaned up immaculately. And when I found warpage issues I learned to pause the cut in various locations to alleviate the situation. Even if it meant after every letter cut. So to me you're not attempting to put in too much detail necessarily but trying too fast with what you have.
Torch height must be consistent. Too high allows more heat to be distributed to the plate. Cutting too slow also adds to warpage so we all understand cutting as fast as possible. Also I'm fairly certain CandCNC would be the electronics running the setup not the machine itself but as stated drawing is more my thing. The water table is one way to keep you from choking to death on the fumes, another is exhaust fan/ductwork.

Take care!

[BTA Plasma]

Looks like a CNC router parts build not CandCNC. Might have some speed settings way off or a lack of power for good acceleration.

[michmetalman]

That is too thin of metal for all those cut outs

[MountainWerks]

Hi Guys. Thank you very much for the feedback. I'll try to get more information on the setup and exactly what it is (equipment, etc.) when the school opens back up in January. I was hoping to be able to download a manual which would be helpful but I couldn't find out what model it was before session was out. Yes, it's running Mach 3 and I've located the setting in sheetcam that adjusts for warpage so I'll use that next time. I don't know how to get the torch to pause between cuts but I'll do some research on that and see what I come up with. Since THC is down, I was going to try raising the water table over the sheet since the ohmic sensor shorting wouldn't be an issue. I'll play with the speed as well Ben. I'm confident it can do this level of detail, it's just figuring out how to get the warpage under control. I've been talking with the local Hypertherm rep and he's shown me some stuff local guys have done that is this tight and flat as a pancake with very little dross.

I have not tried fine cut yet as I understand it's more difficult to dial in than standard consumables. Also, they college kids keep changing the tool settings whenever I come back in so I always have to change them back. (hey you kids, get off my lawn!). I appreciate the feedback and will update when I get more information.

[acourtjester]

" I don't know how to get the torch to pause between cuts"
Here is how you do that, In sheetCam you need to create a new code snippet for an Optional program stop, this is Mo1.
See attached screenshot, you click on the code snippet and this opens up a code snippet window, you name it and put m01 in it and save it.
When you want to put a stop in after each operation you would click on the code icon in the operations window and click OK and it will put one in.
after you have all the operations for your cut routine you do a Post Processor and the g-code will have a stop at each place you inserted one.
don't forget to save the tools for later use.

[djreiswig]

You can save your toolset and reload it when you come back. That'll show them whippersnappers.

[ben de lappe]

Dang whippersnappers... Save and load...and lock if at all possible. Maybe remove a swirl ring on 'em….oops, you know where I'm going here..
Torchmate made it easy to pause between cuts for us. All the Mrs. had to do was press any key to pause the machine at any time, even during a cut. Similar to an E-stop but without losing everything. Pretty much worked flawlessly. I just didn't like to pause in a cut because of the arc divot left behind from start/stop and would wait until the cut was complete.


Tackle the basics as discussed here and you'll be well on your way to improving your warpage issues. By Lightyears...

Thanks for jumping in with the G-Code technical programming knowledge Tom! You technical guys are the best.

[jimcolt]

Warpage and dross are caused by 1. cutting too slow, 2. cutting with the torch height too high, 3. cutting thinner materials with too much power.

1. Use the smallest amperage consumables at the specs listed in the operators manual (plasma cutter manual) for your material and thickness. If you see dross....do not slow down (most beginners do!), go faster.....do a few straight line test cuts at faster and faster speeds (increase by 3 to 5 ipm per test)...eventually the dross will minimize.

2. Be sure your arc voltage based height control is active and operating as designed. Start with the volatages listed in the plasma operators manual cut charts, adjust voltage so that the physical cut height is correct. If the physical height is higher that than the cut chart suggests...then lower the preset voltage until it is correct. This has to be checked periodically because consumable wear will cause the voltage /height relationship to change, as will cut speed changes.

The plasma will not do everything......you must be sure all of the settings on plasma and cnc machine and height control are correct for repeatable, good quality cuts. Jim Colt

[MountainWerks]

Jim, Ben, Tom, Thanks. I'm printing this post out and taking it in the next time I hit the college and I'll let you know what happens. You guys rock! Maybe I'll bring those kids some exlax brownies, they eat anything and everything!

[MountainWerks]

Hi Guys,

Ok, so school is back in session and I was able to get some table time. After discovering that all the tools had been erased in Sheetcam, I set to inputting them again and started cutting and….well.. I discovered after a couple of false starts that someone had put in fine cut consumables…. so I swapped them out with the best standard cut consumable I could find and here are the results. As you can see it’s… not good. Lots of irregularity on the small cuts and pretty much just gouging on any long distance cuts with a lot of spatter.




So, I think this might be a consumables issue, but I’ll share with you the tool settings and see what you guys this. I’m cutting 16 gauge cold rolled and here’s how sheetcam is setup. THC is supposedly working after they swapped out a blown board.








I set this up by the book. THC should set cut height automatically based on tip voltage right? Voltage was set a 1.28


Now on to the consumables, and this is where I think I’m having the issue. Take a look at the electrode.






So, what do you think….?

[djreiswig]

What does the tool settings screen look like for this tool. Your cut height should be 0.06 and voltage should be 125-128 or whatever it takes to keep the cut height at 0.06. Do some straight line test cuts with your THC off and see if your cut height is correct. You could have a referencing issue and be raising to the wrong pierce & cut height. That's what it looks like to me.

[acourtjester]

In image #3 you have the post processor as CNC Router, I would say those consumable have seen better days. The Swirl ring show 857 as the last numbers and that is for a 65 to 85, you have a 45??
Has anybody check the calibration on the table, if the steps per are off this would change the cutting speed too. You may have a situation where to many have played with the table and things are way out of whack. Quick check is to measure the drawing size against the cut size. But it still may need a full calibration.

[WyoGreen]

MountainWerks,

Your picture of the manual page shows it's for a HP45XP, if so that means it's probably a Duramax torch, so the consumables you show are probably right, but they are in poor condition, as acourtjester pointed out. The pictures show several deviations from best plasma practices, such as the plasma cutter work clamp on the slats instead of the material (which can result in reduced cutting current), the plasma cables coiled up under the table (which can lead to noise induction), The controller and cutter under a water table (which can lead to water in both of them). The sheetcam tooltable shows variance in both the pierce height and the cutting height. For Hypertherm units, it should be .15 for the pierce height and .060 for the cut height. That sheetcam tooltable should look pretty much like the page from the Hypertherm owners manual. I'm not familiar with the CNC Router parts controller, but it appears that it uses Ohmic sensing for touch off height control, so perhaps there is a problem with that also.
All in all, I'd say too many people have had their fingers in the system and it probably needs set up right from the beginning. I did go to the CNC Router Parts web page, and they seem to have a lot of information about how their systems should be set up.

Steve

http://www.cncrouterparts.com/instructi ... 337q486tm6

[jimcolt]

I think your consumables look fine for a typical water table application, though you may have some moisture or oil in your air lines. You mentioned early on that there was a "couple of loops of pipe" for a moisture trap.....is there an actual moisture oil separator and drain downstream of that pipe? Water and oil need to be cooled (that is the job of the loops of pipe) and then separated (usually with a coalescing filter with auto drain) to be effective. To determine if oil or water....pull of the plastic float bown from the 45XP plasma and inspect the inside (it has a drain mechanism....but there should be signs of water droplets or oil inside the bowl...if there is some).

Next...it clearly looks like you are cutting far too slow...as indicated by the heavy bottom dross. Get back up to book speeds. Jim Colt

[tcaudle]

I may be wrong but the THC CNCRouterparts uses is a manual setting unit meaning the preset volts has to be programmed into the THC and is not automatic from the MACH3 screen. Its not a CandCNC control or the DTHC. The touch off (called IHS) is critical and needs to be accurate . The mechanical switch on the floating torch holder has to have a "Switch Offset" value that is determined by testing . its different for every machine. The tooltable then will define where the pierce height, pierce delay and cut height are set .

[MountainWerks]

Sorry for the late reply as I have been traveling out of town all week. tcaudle, jimcolt, Wyogreen, acourtjester, djreiswig, thank you for your suggestions and willingness to help. I will check on everything you suggested when I'm there next week. I'll report back!

[djreiswig]

Also check that you are cutting in the proper direction. The arc is straighter on one side of the torch. I always have Reverse cut direction checked on my system.