Cutting corrogated metal

[edclayton1]

Yesterday I decided to take a stab at cutting corrugated metal for my first time. I have managed to successfully cut quite a bit of diamond plate so I figured corrugated shouldn't be too much more difficult. First I read up about it here on Plasma Spider because I knew it was going to be a bit of a project and would require some tweaking to my settings to say the least. I found some good info but most of it was with either different hardware or software than what I am now using but at least the principals should still apply. I am now using the CandCNC bladerunner setup with Linux Command CNC.
First I headed over to the hub ad min and kicked up my velocity and acceleration to higher than the recommended values as shown on the CandCNC setup videos I had previously used on YouTube when I first setup the machine. I tested my setup and did not seem to encounter any issues such as missed steps so I figured that was a good thing, I think I tripled my original values from what they were previously.
Then in sheet-cam I determined that it wanted to use 350 IPM for the X and Y speeds for the 26G material. ( I am working with my Hypertherm 45 on this plasma table) I had read here that it may be helpful to so that down some for a better ratio between the XY and the Z axis speeds. So I slowed it down to 300 IPM on my second attempt. (the first attempt didn't seem to work out with out the torch going both too high away from the work and also crashing into the work at other times.) I also went into the settings for DHTC-IV in the CommandCNC software and changed the radio button to custom as fast also didnt seem to react fast enough to avoid crashing and excessive lifting away from the work. After I selected custom I then slid the controls to 50% for both responsiveness and tracking and increased the voltage tolerance to something greater than default. All this seemed to help but it still turned out to want to contact the metal sometimes and pull too ar away from the work at others.
Sooo, That is what I did, it did make my artwork more or less successfully but I am hoping people here can tell me what all I did wrong and what I should do to get this thing dialed in better for corrugated metal work. I am sure it can do it I just need to learn how to set it up properly.

[tcaudle]

If this is a stepper based Z and the typical 5Pi you are WAY over the max RPM you can expect. To get 350 ipm you have to spin the motor at 1750 RPM. That is 500 RPM than I have ever seen one do reliably. SO roll it back to about 200 to 250 and slow down the feedrate to about the same. You will need to then compensate with slight higher Preset volts. Crank the settings back down to the Fast settings even if you leave it on custom. You cannot have any pierce delay plunge time (so pierce height needs to be .01" higher than cut height) and acceleration needs to be from 50 to 100 and up and down velocity in Hub utility the same. Get the feedrates back down into the 200 IPM range (our video on 26ga was done at 180IPM) with the Z tuned to 250 Do yourself a favor and make a NEW Config and clone the regular stuff. The DTHC settings are not stored in the Config so they will have to change each time you decide to fut flat versus corrugated. You have to make sure things like your touch off limit (in CommandCNC) is more thant the depth of a trough from a peak. its a negative number. Having a feather touch is an advantage because there are fewer settings and less cycle time. Your Rapid height has to be higher that the highest peak. Its not for the faint-of-heart but it is really neat when you can make cut-outs in corrugated without out having to pierce and start on a flat spot to get s sample voltage or to have the delays not kill you if the cut starts in the middle of a rib!.


Raising the gain and tracking makes it less stable and more prone to overshoot. Fast preset is REALLY aggressive.

[edclayton1]

Thanks very much for all the advise. I will make the changes you recommend as best as I can understand. I knew I was winging it but I figured if I posted this is might get some useful feedback to better understand what I need to do. I do have the feather touch but I did notice even with it, it would cause the metal to deflect when I homed the z axis. I chose to start at a high spot to do my initial z homing zeroing but some of the cuts start on the slopes and in the valleys so I didn't know how to deal with that. I also was trying to shorten my dhtc on delay time but it looks like that was the wrong thing to be doing. I was changing it to be .3 sec. Thinking that the sooner it came on the better for going over such a irregular surface. I didnt realize it needed time to stabilize. Back to the drawing board tomorrow. I should probably buy some fine cut nozzles for this thickness material but I hear they are more finicky to deal with too. So I didn't want to make it harder than it was already going to be to get setup. BTW this is a stepper system with the 620 Oz. Steppers and the 5 tp (or 10 times 2)i velox z axis. I wasn't trying to get it to go 350 IPM on the z axis but rather 175 IPM according to someone's recommendation here with 350 for the x and y axis because that's the speed that sheetcam called for for the 26 gauge thickness. (I guess I need to cross check that with my hypertherm chart) but I think I already did that once and it was close or spot on. When I made the change to 300 IPM in sheetcam I assume it was changing the x and y speeds only in the g code.
I don't think I was having an issue with the rapid height but I will change that from 1 inch to 1.5 inches just to be sure. That makes good sense and I don't think I even considered it. Of course it wasn't an issue when I was dealing with the diamond plate and I was able to see the voltage and the z stepper working great when cutting that material. So I have no doubt the dhtciv can do this once I get it adjusted correctly. Also I like your suggestion for making a new configuration for corrugated metal. That's a great idea, too. Thanks again.
Cheers, Ed

[Rodw]

If you stop and think about this, the Z axis maximum velocity becomes the limiting factor. It has to go up and down 1.5" every 1.5" of X or Y travel or thereabouts. If your cutting speed is set at a level beyond what the Z axis can cope with, you will get collisions. eg. My machine can move in X and Y directions about 5x faster than it can on the Z but obviously it can't cut Corrugated Iron at its maximum feed rate.

In other words for example, if the Z can only go up and down a hump every 1 second, you can't feed at 5 humps a second. You need to set the feed velocity at a maximum of 1 hump per second less an allowance for THC and direction changes.

[tcaudle]

Yes. Climbing a 45 deg slope says your vertical travel is is the same speed as the horz. You need to crank the horz back or the z will hit the edge of the slope. In actuality the Z nees to be a little faster than XY . Never forget that your ACTUAL feedrate is a vector sum of the two axis feedrates.

You cannot have any delay in the DTHC coming one. Yes you will get a tiny dive BUT on really thin material the pierce time is almost instant and the voltage spike dies out really quick. If you touch off on on the side of a rise the DTHC has to react instantly.

There shoul dbe no deflection on the ohmic sensor. If it is you need to set the plunge safety clearance higher because it slows down to the touch off speed . Since you never know where top of material is then it can be way off. Set your rapid clearance at least 1" above the top of the peaks and your plunge safety to the same point. It wiil then slow down no matter where the material is (which will slow it down if the material is actually a long ways from the torch tip).

Cutting 26 ga flat material at 350 is no cake walk. cutting corrugated at 350 takes more speed on the Z than waht you can muster with that Z and motor combo.

[edclayton1]

Thanks again to all for the info. I will add this to my notes and apply these suggestions to the settings.
There is so much to learn but its really interesting. Its slowly starting to sink in I think.
Cheers,
Ed