Z axis problems

For general topics and questions that do not fit into any of the other categories or forums.
Post Reply
BensPlasmaAu
2.5 Star Member
2.5 Star Member
Posts: 209
Joined: Mon Jan 13, 2014 10:37 am
Location: Boronia, Melbourne, Australia

Z axis problems

Post by BensPlasmaAu »

Hi all. I have finally gotten myself up to the stage of tuning in my motors and getting a few dry runs in. I am having a problem with the z though. I have set up a floating torch holder. The torch comes down lifts up the holder and clicks off the z home microswitch. It then heads back upwards briefly and stops. It does not actually lift the torch off the surface of the material, and it also doesn't reference the height to zero. I seem to have to do that myself. Can someone let me know if this is the correct way of things happening or do I need to find an option buried in Mach3?

My machine is a home built job, running Candcnc Bladerunner DTHC IV.

Any help would be greatly appreciated.

Ben
KIDTech
3 Star Member
3 Star Member
Posts: 359
Joined: Tue Oct 28, 2014 1:21 pm

Re: Z axis problems

Post by KIDTech »

I can't say anything for the CandCnc stuff as I do not have that but I can tell you how mine works. Mine triggers the switch, moves up to let the switch out, zeros, then moves up the the spot where the torch will be lifted from the material and zeros again. I hope this helps, I use SheetCam and this has worked really well for me. Let me know if you would like any other help.
DIY 5x10 v rail, rack and pinion
Gecko g540
Pm65 - aka game changer
Longevity ForceCut 42i is sitting on the shelf
Proma THC
ACAD, SheetCam, Mach3
Millermatic 211
NEW HORSE IN THE STABLE:
4'x8' LDR downdraft w/a scribe
Milltronics Partner 2 CNC mill
User avatar
acourtjester
6 Star Elite Contributing Member
6 Star Elite Contributing Member
Posts: 7770
Joined: Sat Jun 02, 2012 6:04 pm
Location: Pensacola, Fla

Re: Z axis problems

Post by acourtjester »

This is a function of the G-code and the electronics you did not state that you were doing this under a g-code.
here is what mine looks like with a DTHCIV from CandCNC.
N0200 G00 Z1.000
N0210 X0.526 Y9.412
N0220 M900 (Check for Z active)
N0230 G28.1 Z0.02 (Start Touch-Off )
N0240 G92 Z0.0
N0250 G00 Z0.027 (Switch Offset Lift)
N0260 G92 Z0.0
N0270 G00 Z0.1500
N0280 M03
N0290 G04 P0.4
N0300 G01 Z0.060 F30.0
DIY 4X4 Plasma/Router Table
Hypertherm PM65 Machine Torch
Drag Knife and Scribe
Miller Mig welder
13" metal lathe
Small Mill
Everlast PowerTig 255 EXT
mike 1948
2 Star Member
2 Star Member
Posts: 66
Joined: Wed May 08, 2013 11:23 am

Re: Z axis problems

Post by mike 1948 »

First off, I don't know anything about the DTHCIV. Here is how I use a Sheetcam post to setup my torch switch offset. Bring the torch down manually until it just touches material. Zero the z axis, then continue to lower the torch until the switch trips, record the z axis DRO and put this amount into the "switch offset" in the post processor. With the correct switch offset the torch should lift off the material
Not sure if this applies in you situation.

Mike
vatso
1 Star Member
1 Star Member
Posts: 19
Joined: Thu Oct 23, 2014 11:00 am

Re: Z axis problems

Post by vatso »

BensPlasmaAu wrote:Hi all. I have finally gotten myself up to the stage of tuning in my motors and getting a few dry runs in. I am having a problem with the z though. I have set up a floating torch holder. The torch comes down lifts up the holder and clicks off the z home microswitch. It then heads back upwards briefly and stops. It does not actually lift the torch off the surface of the material, and it also doesn't reference the height to zero. I seem to have to do that myself. Can someone let me know if this is the correct way of things happening or do I need to find an option buried in Mach3?

My machine is a home built job, running Candcnc Bladerunner DTHC IV.

Any help would be greatly appreciated.

Ben
What Post Processor are you using in sheet cam I had an issue like that once
User avatar
steel 35
3.5 Star Member
3.5 Star Member
Posts: 634
Joined: Sun Jan 11, 2015 11:12 am
Location: N of Cali.

Re: Z axis problems

Post by steel 35 »

Feather touch / Ohmic sensor connections all good? Check them in the Mach Diagnostic page, should light up the correct light on contact with clean grounded surface.
PPL HDG 4X8
Hyp 65 duramax's
C&CNC 620-5 Ethernet
Inkscape, Solid Edge, Sheetcam, Autocad 2K
Corel X7 Student NO DXF!
EasyScriber
BTA Plasma
3.5 Star Elite Contributing Member
3.5 Star Elite Contributing Member
Posts: 590
Joined: Thu May 12, 2011 4:28 pm

Re: Z axis problems

Post by BTA Plasma »

Floating Z with DTHCIV requires you to set the switch offset in Sheetcam Options/machine/post processor and click the box "set custom post options" and change the value from zero to at least .050 for your switch offset.
tcaudle
4 Star Elite Contributing Member
4 Star Elite Contributing Member
Posts: 1353
Joined: Tue Feb 28, 2012 6:47 pm

Re: Z axis problems

Post by tcaudle »

DTHC is not involved in the touch off sequence. All happens in G-code from SheetCAM. Post processor automatically puts in the whole sequence that goes like this:

move to the first pierce point and REF the torch down using a G28.1. Slow down the move at the value given for Z in that command
Zero the MACH DRO using the G90 Z 0.00 command
lift up the SwitchOffset distance (this comes from the value you put into the swtichoffset in "Set Post Processor Options"
How often it does the sequence is based on the total XY travel inches (RefDistance)
Raise the Z to pierce height
Fire the torch
Plunge to Cut Height
Turn on DTHC
Start a cut in XY
BensPlasmaAu
2.5 Star Member
2.5 Star Member
Posts: 209
Joined: Mon Jan 13, 2014 10:37 am
Location: Boronia, Melbourne, Australia

Re: Z axis problems

Post by BensPlasmaAu »

Thank you all so much. I've learned so much off this site through everyone, and I'm still learning now. I have just been trying to get the machine to run around using the scorpion .tap file that comes with the Candcnc electronics. I haven't gotten into sheet cam yet. That's probably the whole bunch of issues I'm having. Thanks again, and keep posting and reading, I'm sure to have a myriad of questions in the coming weeks and months.
BensPlasmaAu
2.5 Star Member
2.5 Star Member
Posts: 209
Joined: Mon Jan 13, 2014 10:37 am
Location: Boronia, Melbourne, Australia

Re: Z axis problems

Post by BensPlasmaAu »

I'm using sheetcam as my post.
vatso
1 Star Member
1 Star Member
Posts: 19
Joined: Thu Oct 23, 2014 11:00 am

Re: Z axis problems

Post by vatso »

BensPlasmaAu wrote:I'm using sheetcam as my post.
Sorry Ben which sheet cam post processor - I use the MP 1000-THC one
BensPlasmaAu
2.5 Star Member
2.5 Star Member
Posts: 209
Joined: Mon Jan 13, 2014 10:37 am
Location: Boronia, Melbourne, Australia

Re: Z axis problems

Post by BensPlasmaAu »

a court jester - where should I be looking for this script? I am using the DTHC-HYT-TAP_SoftPierce+Marker-rev11D post processor.

I loaded a CAD file in, set the tool path and pierce points etc. I ran through a simulation and it goes direct to the first pierce point with a rapid height of 5 mm, then drops the z to 1.5mm pierce height and starts cutting. The z never goes all the way to touch off and then back up to my designated switch offset before getting the correct pierce height and cutting. It seems to just ignore the fact I entered in the switch offset.

Hopefully you know what I mean........ do I have to enter in all that code to make the floating head work?

I have everything set and ready to go with my dry runs, but without sorting this I am dead in the water.
BensPlasmaAu
2.5 Star Member
2.5 Star Member
Posts: 209
Joined: Mon Jan 13, 2014 10:37 am
Location: Boronia, Melbourne, Australia

Re: Z axis problems

Post by BensPlasmaAu »

OK, have found the offset for the z home switch on the floating head. I've done the simulation and it doesn't seem to like to work correctly. Perhaps I am doing things wrong? If I load the .tap file into Mach3, will this then add the code needed to make the floating head touch off work?

Confused, and a little frustrated. But I can't wait to have the thing working!!! Bring on the information!

Thanks again all, I apologise for random thoughts and ideas spilling out into the forum......

Ben
User avatar
acourtjester
6 Star Elite Contributing Member
6 Star Elite Contributing Member
Posts: 7770
Joined: Sat Jun 02, 2012 6:04 pm
Location: Pensacola, Fla

Re: Z axis problems

Post by acourtjester »

HI Ben
The touch off routine is generated by sheetcam when you enter in the correct numbers for it to use. This is done automatically by the post processor used and that is why you need to use one from CandCNC when using their electronics.
Tom’s description of the touch off function is how it should work maybe you needed to just do one step at a time. If I read your statement correctly it is not touching the metal in the first part of the routine to set the pierce height is that correct if not try this.
In mach go to the diagnostics screen and down near the bottom there is a line where you may enter code one line at a time called “Direct G-code Input”. Make sure the reset is not flashing and enter “G28.1 Z0.02 f20” This will move the Z down slowly until it contacts the top of the metal when you hit the enter key. The f20 is just so it will move slowly also when in the diagnostic screen you cannot use the keyboard to move any table motor. This line on the diagnostic screen is just for entering in a command and executing it, to use the keyboard to move just go back to the program screen. You can enter in other commands there and watch what happens one step at a time.
When looking at G-code the “N0XXX” that you see are line number after the space is the actual G-code commands. This is so you know which line to go to if you wants to start the g-code in a place other then the start. When you do this you must move to the line before and hit the “set next line” button and then run. You do not need to move the table to any coordinates it will move to them by using the G-code as long as you don’t zero then out before. After looking at G-codes and seeing the table move things start to make sense.
DIY 4X4 Plasma/Router Table
Hypertherm PM65 Machine Torch
Drag Knife and Scribe
Miller Mig welder
13" metal lathe
Small Mill
Everlast PowerTig 255 EXT
BTA Plasma
3.5 Star Elite Contributing Member
3.5 Star Elite Contributing Member
Posts: 590
Joined: Thu May 12, 2011 4:28 pm

Re: Z axis problems

Post by BTA Plasma »

You should say what you are running first. What electronics?
BensPlasmaAu
2.5 Star Member
2.5 Star Member
Posts: 209
Joined: Mon Jan 13, 2014 10:37 am
Location: Boronia, Melbourne, Australia

Re: Z axis problems

Post by BensPlasmaAu »

Thanks again everyone.

I got the z axis going great. touch off working, pierce height OK etc. So then I discovered everything wasn't that great and the problems started compounding. I went back to the CandCNC website and discovered that there was a whole other manual for setting up the DTHC . I looked for more information on the disc, but I didn't find it. Anyway, I have a heap more info downloaded, and made some discoveries that when I look back at them now I think "What an idiot". Oh well it's all learning. For instance, a Hypertherm Powermax 45 doesn't have a TAP (hope my lingo is right) function where the computer changes the air pressure and the AMPs. Turns out that the plasma was set at 25 AMPs on the dial. SO that obviously didn't want to work properly and kept dropping out with torch volts below spec (or similar fault). The cuts it did do were a bit messy and the holes weren't really round - so I am putting this down to the acceleration as being too low. The gantry and mechanics are solid. I went and drilled and roll pinned every gear and timing pulley on it, and ensured that the belts were the correct tension.

Going through all the setup of the DTHC IV I have come across a few problems. I've posted them on the CandCNC forum anyway, but I thought seeing as there is a wealth of information here I would ask as well.

Some information about my system. Home built table and gantry CandCNC Bladerunner ESP II 620/4, 3:1 belt reduction drives onto a MOD2.0 gear rack with 20 tooth pinions, C3BUS, DTHC IV, hypertherm powermax 45. Mach3 and sheetcam. I have done all the tests up to the PWM bit according to the DTHC installation manual off the CandCNC website.

Testing the PWM voltage. I push the test button, the LED flashes and I get 124 volts at torch displayed on the Mach3 screen (meant to be 126 -128) I'm hoping that is Ok being 2 volts out??? When I push the button again the LED goes out and the volts at torch goes to 45.

1. Is 124 volts within spec only being 2 out?
2. How do I calibrate the PWM to get it within spec if I need to?
3. Why do the volts stay at 45 instead of dropping to 0?
4. How do I fix this?

From here I'm pretty sure that there are going to be a few tweaks and amendments to things, but I should be getting close. Thoughts, comments knowledge. Throw them at me :)

Ben
BensPlasmaAu
2.5 Star Member
2.5 Star Member
Posts: 209
Joined: Mon Jan 13, 2014 10:37 am
Location: Boronia, Melbourne, Australia

Re: Z axis problems

Post by BensPlasmaAu »

acourtjester wrote:HI Ben
The touch off routine is generated by sheetcam when you enter in the correct numbers for it to use. This is done automatically by the post processor used and that is why you need to use one from CandCNC when using their electronics.
Tom’s description of the touch off function is how it should work maybe you needed to just do one step at a time. If I read your statement correctly it is not touching the metal in the first part of the routine to set the pierce height is that correct if not try this.
In mach go to the diagnostics screen and down near the bottom there is a line where you may enter code one line at a time called “Direct G-code Input”. Make sure the reset is not flashing and enter “G28.1 Z0.02 f20” This will move the Z down slowly until it contacts the top of the metal when you hit the enter key. The f20 is just so it will move slowly also when in the diagnostic screen you cannot use the keyboard to move any table motor. This line on the diagnostic screen is just for entering in a command and executing it, to use the keyboard to move just go back to the program screen. You can enter in other commands there and watch what happens one step at a time.
When looking at G-code the “N0XXX” that you see are line number after the space is the actual G-code commands. This is so you know which line to go to if you wants to start the g-code in a place other then the start. When you do this you must move to the line before and hit the “set next line” button and then run. You do not need to move the table to any coordinates it will move to them by using the G-code as long as you don’t zero then out before. After looking at G-codes and seeing the table move things start to make sense.
That's so helpful. I have been starting to understand the g-code as the machine moves around. Code for zero-ing the z, firing the torch etc have become clear as I've fumbled my way through.
User avatar
acourtjester
6 Star Elite Contributing Member
6 Star Elite Contributing Member
Posts: 7770
Joined: Sat Jun 02, 2012 6:04 pm
Location: Pensacola, Fla

Re: Z axis problems

Post by acourtjester »

Ben
For testing purposes you can leave the plasma off and click on the green button “DTHC Auto/Manual” to manual mode then you can run a G-code and watch it do all its moving around.
This may help you to check G-code and learn what it is doing with out burning up metal.. If you make a spring loaded pen you can mount it to the torch and put paper on the metal surface and actually see the G-code draw out the parts. Not something you must do but can help to ID a problem later.
Things are going to start being fun! :D :lol:
DIY 4X4 Plasma/Router Table
Hypertherm PM65 Machine Torch
Drag Knife and Scribe
Miller Mig welder
13" metal lathe
Small Mill
Everlast PowerTig 255 EXT
User avatar
WyoGreen
4 Star Member
4 Star Member
Posts: 897
Joined: Tue Mar 04, 2014 8:36 pm
Location: Cheyenne, Wyoming

Re: Z axis problems

Post by WyoGreen »

Ben, if I remember right, 124 volts is not a problem, I think mine also read 124 volts. There is a procedure to adjust it in the CandCNC manuals, but I wouldn't worry about that right now.

As far as the 45 volts, I just can't quite remember that one. It seems like I did have that occur, but once everything was up and running, it stayed at 0 volts unless I'm cutting.

It sounds like you're ready to start cutting. Like was mentioned, run a tap file with the torch turned off and DTHC turned off and make sure the machine is making the motions it should to cut your part out. If it does , run it with the torch on and DTHC off so see how it cuts. If that works ok, then turn on the DTHC and see how that works out. It seems like that's when people need to do a little tweeking with cut rules in Sheetcam to get everything dialed in and cutting good.

I cut a lot of small circles and squares getting my system dialed in, but it's working great now. I get a little hic-up once in a great while that makes me scratch my head a little, but the guys on here and on the CandCNC site usually get me going again.

Good luck, Steve
Precision Plasma gantry
CommandCNC Linux controller w/Feather Touch & PN200 hand controller
HT-45 plasma cutter
Plate Marker
Router
Laser
User avatar
acourtjester
6 Star Elite Contributing Member
6 Star Elite Contributing Member
Posts: 7770
Joined: Sat Jun 02, 2012 6:04 pm
Location: Pensacola, Fla

Re: Z axis problems

Post by acourtjester »

one thing you do want to do is when setting up the tools for you torch make sure in the box labeled DTHC delay -sec put in about 1.5 these is the delay that hold off the DTHC from reacting to the arc voltage for the time in the delay. After the 1.5 sec the DTHC comes on and will start checking the arc voltage as it is cutting. If not the torch may dive down and it will stop cutting. This needs to be done in every torch setting you have (different metal thickness)
DIY 4X4 Plasma/Router Table
Hypertherm PM65 Machine Torch
Drag Knife and Scribe
Miller Mig welder
13" metal lathe
Small Mill
Everlast PowerTig 255 EXT
BensPlasmaAu
2.5 Star Member
2.5 Star Member
Posts: 209
Joined: Mon Jan 13, 2014 10:37 am
Location: Boronia, Melbourne, Australia

Re: Z axis problems

Post by BensPlasmaAu »

Thanks yet again. Will have to have a go at turning the torch off and running the g-code. I was trying to figure out how to do that, then I just turned to the fiancé and said "Bugger it, i'm going to go make some sparks and fix things that go wrong later." probably not the wisest of moves heading in like a bull at a china shop, but hey, it made sparks and caused many a fist pump!

I was wondering if anyone might be able to share their acceleration values in Mach3 motor tuning? Not sure whether it will be useful because everyone's table seem to be slightly different.
User avatar
acourtjester
6 Star Elite Contributing Member
6 Star Elite Contributing Member
Posts: 7770
Joined: Sat Jun 02, 2012 6:04 pm
Location: Pensacola, Fla

Re: Z axis problems

Post by acourtjester »

The beat way to do motor tuning is to download the demo version of Mach3 from the web and turn off the E stop switch by putting a 0 in the port selection as mach will not turn off the reset with this enabled. Then place the axis you and to work on to the most negative point of its travel then go into settings (top line menu item) in the lower right is a place to select either inch or MM’s select which you want to use. On the table measure to the other end of the axis travel so you will know how far it travels. And down next to the reset is “set step per unit)and click on it. This brings up the axis calibration X is always set if not doing X change to the axis you are using. Click on OK the brings up another menu enter in a value for the distance you want to go (go small at first) hit enter and that table axis will move. Measure how far it went and enter that in the box. Mach3 will calibrate the steps per for you and enter it into the correct location. Repeat this a few time going longer distances each time this will give you a more actuate value to mach to use. When finished with X move to Y then to Z and repeat for them. If you are using 2 motor for one of the axis then go to config menu and go down to “slave axis” and enter the slave axis under the master axis (like X master is slave with B) click in the slaved button. Then enter the new setting for the axis that you are slaving in to the motor tune values for the slave axis.
In the motor tune for each axis you can now work on the velocity and acceleration numbers while test the axis travel.. The acceleration number will be about ¼ the value of the velocity value. You can use the 4 arrow and for X and Y movement and pu and pd for the Z movement for testing. Increase the values until the axis moves faster but does not lock up and vibrate.
There are youtube videos showing this too.
have fun
Tom
DIY 4X4 Plasma/Router Table
Hypertherm PM65 Machine Torch
Drag Knife and Scribe
Miller Mig welder
13" metal lathe
Small Mill
Everlast PowerTig 255 EXT
fabricator909
1 Star Member
1 Star Member
Posts: 18
Joined: Sun Jun 23, 2013 6:38 pm

Re: Z axis problems

Post by fabricator909 »

Hate to bring up an old thread, but it has very useful information, and our problem is somewhat similar on our machine.
Machine Specs:
CandCNC Dragon Cut Servo Ethercut & DTHCIV
HYT Advanced Connection Kit
PC came from CandCNC with software installed
Servos are direct drive on .75" Pinion- Calculated Steps 4244
Machine is on machined rails, both x and y axis

We are in the motor tuning stages as well, however our Z-axis wants to plunge through the material even once it has it the limit switch on the floating head. We have the switch wired to the ohmic sensor as described in the manual, although the ohmic option is something we will very rarely use IMO because we will be cutting 11ga and up material most of the time. We have tried NO and NC positions on the switch (the manual contradicts itself on switch position). At a loss at the moment on what the problem is, we also tried the G-CODE acourtjester posted, to maybe see if the switch only worked with g code, but it didn't work.
User avatar
WyoGreen
4 Star Member
4 Star Member
Posts: 897
Joined: Tue Mar 04, 2014 8:36 pm
Location: Cheyenne, Wyoming

Re: Z axis problems

Post by WyoGreen »

Fabricator, there are several ways to wire the Ohmic sensor and the Z floating switch. The Ohmic sensor will be used to sense the top of the metal, irregardless of what gauge it is. The plasma cutting process requires a very narrow range of heights above the metal, so the system needs to know where the top of the material is before every job.

The Z floating switch can be used a couple of different ways. It can be used to back up the Ohmic sensor, it can be used as a limit switch, and it can be used as an E-stop with the Ohmic sensor. It is usually recommended that you get your machine running without the Ohmic sensor at first, just using the Z switch as the material top sensor. Servo's need limit switches to keep from hitting the stops and stalling, which can damage them. Steppers don't care if they hit the stops, they just make a bunch of racket without damage.

At any rate, it would be helpful if we knew what operating system you are using, Mach3 or CommandCNC (Linux). Then we can advise some wiring and testing steps.

Steve
Precision Plasma gantry
CommandCNC Linux controller w/Feather Touch & PN200 hand controller
HT-45 plasma cutter
Plate Marker
Router
Laser
fabricator909
1 Star Member
1 Star Member
Posts: 18
Joined: Sun Jun 23, 2013 6:38 pm

Re: Z axis problems

Post by fabricator909 »

Wyogreen, thanks for the quick reply. We are running Mach3. At this point, we would rather get up and running without using the ohmic sensor honestly.
Post Reply

Return to “CNC Plasma Cutters General Forum”