LinkBack URL
About LinkBacks
This does sound like a THC problem. How is your piercing? Is the torch piercing from the correct height and then lowering itself during cutting? I'm not sure about yours, but my pierce distance is usually about double my cutting distance.
| | |
I've got a part with 14 cuts in it. The first few cuts seem to work fine, but by what almost seems like an increasing increment the plasma torch keeps getting closer and closer to the work piece. By the time it gets to the 5th or 6th cut, the torch tip is actually touching the metal. By the 7th cut or so, I have to stop it, manually lift the Z off the metal and start it up again. If the THC was working correctly, shouldn't it be preventing that? Does that sound like a THC issue or something else overriding it?
Thx.
This does sound like a THC problem. How is your piercing? Is the torch piercing from the correct height and then lowering itself during cutting? I'm not sure about yours, but my pierce distance is usually about double my cutting distance.
Sounds like a problem with the material referencing. You have some kind of a floating head? does it seam to refrence ok each time? It could be as simple as adding some more referencing G28's in your gcode or it could also be some of settings if you are using Mach3. If you are using Mach I can tell you a couple things to look for.
Jeff T.
http://www.3dcarvestudio.com
Yes, it has a floating head. It's using sheetcam, an MP3000 and Mach3. I'm still wet behind the ears with this stuff, but from what I've come to decipher, before it starts a new cut, it's using the following code:Originally Posted by jeffery71
N010 G28.1 Z0.12
N020 G92 Z0.0
N030 G00 Z0.4900
N040 G92 Z0.0
N050 G00 Z0.1800
N060 M03
N070 G01 Z0.1400 F25
I know I probably don't need to know this, but if you'll humor me a sec; line 10 tells the floating head to find the home switch attached to it and soft stops .12? But I don't really understand why it changes the coordinate system next. Just as an aside, I would appreciate it if you are someone could explain this to me a little better. I'm guessing M03 is being used to fire the torch?
Anyway, thanks.
N010 G28.1 Z0.12
N020 G92 Z0.0 (zeros out dro in Mach)
N030 G00 Z0.4900 (torch offset - raises torch to clear metal barely)
N040 G92 Z0.0 (tells Mach torch is at zero and resets dro)
N050 G00 Z0.1800 (raises torch to pierce height)
N060 M03 (fires torch)
N070 G01 Z0.1400 F25 (torch moves to cut height at feed speed of 25)
Hope this helps some.
Yes, it does help... a lot! Thank you very much.
Oh, one last thing. Line 30, what's telling the machine .49" clears the metal? How does it determine that?
Couple things. First in Mach3 Check under "Ports and Pins" Click the "Mill Options" tab.. Make sure "allow THC up/down control even if not in THC mode" is NOT checked. Your THC will not work properly if it is. This can cause your torch to progressivly get lower or higher.
Do you know how much your switch offset is? or lost movment whatever you want to call it. In the Gcode you posted N030 G00 Z0.4900 That is allowing for .49" offset.
Check those two things first see if that is the problem
Jeff T.
http://www.3dcarvestudio.com
Yeah, I just went and measured it. I think I get it now. =) The .49" is the distant of travel on the floating head from the bottom of its movement to the point where it triggers the switch (I will understand this stuff eventually, by god). I'll check the other setting and see if that's the case and helps.
Thanks a lot.
The other thing to check is if the Z DRO does not agree with the actual height at the end of a cut. This is a strong indicator that the Z is losing steps during the cut. It will continue to try and adjust adding in steps (which is why encoder feedback on a stepper for position correction does not work) so the DRO "thinks"it is higher than it really is and moves it too low on the next pierce. First thing to check is the THC rate in MACH. If it is above 30% try reducing it to 30%. The number is the percentage the Z moves during THC of the MAX velocity. Since no accel or decel curves are added to THC moves it's easy to stall the motor if you try to move too fast. It won't stall during normal moves(jog) because it uses normal Accel curves. The default percentage is a guess because every Z is different. You wnat to run as high as you can speed wise on the Z but if the resolution is to course you get overshoot and a condtion called head bounce. You can usually tame it with lowering the THC RATE setting. There are DTHC settings in the CUT PROFILE that need to be adjusted if you use different nozzle sizes and different thicknesses of materials
The switchoffset value is explained in the DTHC manual and how to set it in SheetCAM so it's automatic on the touch off. There really is a lot of information in the DTHC manual about how to setup, test and cut with plasma including a couple of pages on "how a THC Works".
The support site will get you pretty quick response. I have that coming into my mail box and I check it after hours and on weekends.
I like using the support Forum because it helps multiple users at the same time and it saves me from answering the same questions over and over. I try to take as many calls as possible and answer e-mails but I put a lot of effort into the manuals ( I know, I know, it's overwhelming when you are first starting out) and usually the answer is in there. Not trying to make excuses but it gets pretty crazy in the shop this time of year and it seems like almost everything needs some level of my involvement! So if you try the manual first then the support forum and STILL can't get it to work then call. Usually I can get it done on the Forum and it helps us both (and maybe others).
So here I am at midnight in Texas on a Saturday night reading CNCZone.....Gawd, I have no life[but, I LOVE my job]
TOM Caudle
www.CandCNC.com
Thank you for the information, sir. I was not aware of a DTHC manual. I'll add it to my reading list. The people that sold this machine to my friends left 3 letter-sized pages of instructions on how to run it. lol. The instructions were basically as follows: Open cad software, draw part; open sheetcam, move things to layers, define inside/outside cuts; Open mach3, load g-code, push thc button, click run... easy as that.
Ah huh. Sure. Right. No more complicated than a big toaster. Just stick the metal in and pop out a part.
All of our manuals are on the CandCNC website http://www.CandCNC.com/manuals There are over 100 pages of manuals on just the MP3000 and the DTHC expansion module. The steps you describe are pretty much the basics and once things are tuned and setup it becomes about that easy. So is flying a plane after you have done it for along time (:')
We also maintain a full time support forum (CandCNCSupport Yahoo Forum) that is open to all our customers and anybody interested in building thier own CNC machine or retro fitting an existing machine. We give support on all of our products regardless of who sold them or how the current owner came to be in possession. If you have purchased a complete machine from a vendor we ask you contact them first because it may be a mechanical problem we can't fix. They are responsible for level one questions and contact us on suspected electronic or DTHC issues. If they fail to get the problem fixed we are here. If your vendor has folded or you are not the primary owner you may not get the direct support you need so once again we are here for our electronics. We do not always furnish complete systems (i.e. Controller, Drives, motors, etc) to the vendors so our support may only be up to a point but after hundreds of installs and seeing most issues we can usually point you to the area to test or replace.
Tom Caudle
www.CandCNC.com
It's just amusing to me. It's how I got my first job. The one I've had for the last 15 years. Someone sold a printing company an imagesetter and told them it would be a snap to run. I knew a little about computers and because my dad worked there they hired me to "see them though the transition". Whatever. I've been there ever since. It is never as simple as the salesman claim.
It's kind of like a doctor showing someone else how to preform a tracheotomy and then sending them out into the world. It's a pretty simple procedure, and seven times out of ten, maybe it works just fine, but the other three times something goes horribly wrong and without a complete background in medicine, you don't know what the hell to do at that point.
I see this being much the same thing. These guys bought this thing, and sure, it's supposed to be "that easy", and most of the time maybe it is, but it's those other three times (when you are under the gun and backed up against deadlines and obligations and you are supposed to produce something, but your machine is all jacked up) that you start wondering what you got yourself into. Without a rudimentary understanding of what you are dealing with, if things go all off course, you're screwed. You either have to know things things or hire someone who does.
Posting Permissions
| | |
