Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: jeremyrockjock on May 04, 2011, 06:44:10 PM
-
After a reinstall of mach3 and THC300 the torch is moving out to the first cut and then moves up instead of down to touch off. I have the motor direction set correctly and it bumps up to jog as it should. Any ideas what it is? I am using sheetcam to process gcode.
-
After playing around more I found that reverse z axis under home/limits did the job.
-
I'm guessing you're using "home" touch off (as opposed to G31). Although what you've done obviously works, I'm guessing you have "home negetive" ticked as well which is kind of a double negetive way of doing things if you see what I mean. You could just have set set "home positive" i.e. home downwards.
Ian
-
I have a floating head and am using a switch on z home input. I have read about the g31 somewhere but i am not sure what it is or how it works. If there is a better way I sure would rather do it.
-
I cannot figure this out. Can someone explain what is g31 and how do I set it up? What is happening is the head is coming down to make the home z switch, zeros out the dro and then pushed harder into the metal for the Peirce height is stead of coming up. Also it is not doing my post variable offset even though I have set it in sheetcam.
-
Can you post a short section of your code that shows the HomeZ routine?
It sounds like you have problems with the Zhome switch sticking. Double check the function in the diagnostic page. Watch the Zhome led and trip the switch by hand. See that it changes state. Next make sure the state is what you need in your setup.
(;-) TP
-
I found the g31 code processor in sheetcam and set it up. Now the torch is coming down to touch off and continues to drive into the plate. Under the g31 control should the input for the touch off switch be set on a different input? Mine is set on z home port 1 pin 13
How do I post my code?
-
z home switch is working fine. I just have something ticked wrong
-
Open the code in notepad Copy a section of code then paste it into the reply window.
I would get it working with the zhome then when it is working ok switch IF you want. Here it works equally well either way. Six of one half a dozen of the other.
(;-) TP
-
Question, If you set your Z to zero then from the MDI issue a G1 Z-1.000 F5, which way does the head go Up or down?
Just a thought, (;-) TP
-
If I issue g1 z-1.000 in the mdi the torch moves down. I have set my varible offset at .275 and pierce height at .100 but I don't see them in the code.
Here is the first part of the code.
N0000 (Filename: Roof Rack clamp HWE style scaled up.tap)
N0010 (Post processor: Plasma THC300 - G31.post)
N0020 (Date: 5/8/2011)
N0030 G20 (Units: Inches)
N0040 G53 G90 G40
N0050 F1
N0060 S500
N0070 (Part: Roof Rack clamp HWE style scaled up)
N0080 (Process: Plasma, 0, Plasma, 0.0008 inch kerf)
N0090 M06 T0 (Plasma, 0.0008 inch kerf)
N0100 G00 Z0.1575
N0110 X-0.1600 Y-0.1604
N0120 G31 Z -100 F19.685
N0130 G92 Z0.0
N0140 G00 Z0.0000
N0150 G92 Z0.0
N0160 G00 X-0.1600 Y-0.1604 Z0.1000
N0170 M03
N0180 G02 X0.0000 Y-0.0004 I0.1600 J0.0000 F60.0
N0190 G01 X1.0400
N0200 G03 X1.0404 Y0.0000 I0.0000 J0.0004
N0210 G01 Y3.1200
N0220 G02 X1.9896 Y3.1200 I0.4746 J0.0000
N0230 G01 Y0.0000
N0240 G03 X1.9900 Y-0.0004 I0.0004 J0.0000
N0250 G01 X3.0300
N0260 G03 X3.0304 Y0.0000 I0.0000 J0.0004
-
Also When I run the processor it says I have 0 on the feed rate and the plunge rate but I have set both of those to 30 and 50 prior to running post processor.
-
If you are going to use the G31 you MUST set up your Zhome switch as a probe and setup the port/pin for the probe.
Also your setbacks are not set for the pull back on the head after it homes. You must test your setup to determine the proper pullback to account for switch movement and flexure of the material. If you have to keep adjusting the allowance until it IS what it say it is.
I would slow down the plunge rate untill you get used to the process it is very easy to tear the head off if you get it hung up.
IF the post says 0 feedrate then you need to reset it to the correct speeds.
ALSO your code show the Kerf width as .0008 (;-) You need to set it to the correct amount , normally around .060-.080" works here.
That should get you started, (;-) TP
-
Are you saying use the "probe" in the inputs and set to the pin I have for the z home switch which is 13. If so I tried but it does not respond when I make the switch. However I know the switch work because it shows under z home input if I set up the pin under that.
I setback is set but sheetcam is not processing it. Same with the pierce height and the feed rates. Its like the latest sheetcam software is a dud. It will not process my changes.
-
I am using the same Sheetcam software and there is nothing wrong with it. (;-)
Where are you setting the setback? it is set inside the Post you have to use edit to set it.
The feedreates are set in the tool settings for the selected tool.
The probe sets up with the same port/pin you used on the Zhome. You turn OFF Z home. Then turn ON the probe. When you click the switch you should see the input for the probe light up as you did the Zhome . You should NOT see the Zhome light up any more.
What post are you using ??
(;-) TP
-
I think my sheetcam issues might be attributed to the fact that I lost my licence file when I hard drive crashed. I email them to get a new copy.
I turned off the z home input and set the probe input to the proper port/pin but it was not reading the switch. I even tried automatic setup.
I am using post processor Plasma THC300 with G31
-
You need to figure out the input problem .IF it worked with Zhome it should work with the probe. Double check your Port/pin settings, make sure the probe input is checked active.
Are you in demo mode with MACH??
(;-)TP
-
OK i just tested the Post and it works fine IF you have the setback set other than 0.
You are editing the post to set the setback correct?
(;-) TP
-
Okay. I finally got a response for input "probe Switch" and set it for my touch off switch. I reloaded sheetcam, added the license file and it will still not generate the code for the varible offset. Whill sheetcam not autogenerate all the code I need to run g31 or will I have to edit every file I create?
I am running a licensed mach3.
-
I don't think the problem with the offset is in sheetcam. When I load the code in mach it flashed (error post varible torch offset =.27)
Mach does not like my offset code.
Although when I look at my code in notepad it does not show the offset value. I am so confused. ???
-
Everything seems to be working right except that mach is not using my varible torch code. Also How do I get the torch to touch off and zero more often between cuts?
-
YOU have to EDIT and modify the POST PROCESSOR to change the offset distance. As long as it is set to zero it will NOT generate the offset code.
Also you change the distance for rehoming in the post processor. Normal setting is 500mm, after 500mm of cutting moment it will issue the code to rehome at the next pierce.
"varible torch code" DOn't know what you are meaning to say here.
(;-) TP
-
At the top of sheetcam I click onoperation, set post varible and plugged in .270 inches. After I hit post processor I then open that .tap file in mach3 and it said in the error line process: post varible torch offset =.27
If I continue to run the code it will not do the torch offset but will instead stop at the peirce height. It ignores the setback value. Is there something in gen config that will tell mach to ignore it?
On the rehoming, do I change that under the options, machine options, post processor and click on the edit post botton?
I do apprecatie your help. My machine was running good before the crash and it was setup totally different from this so I am relearning it again.
-
YOu DO NOT USE set post variable to set the offset distance.
You must open the Post code itself with edit and then modify the line that sets the offsetting.
Go to Machine, Post, and select the post your are using. then OPEN the file with the edit button. Curser down to the operation section and you will see a note(green highlighted) that shows you what to modify to set the offset value.
(;-) TP
You also set the rehome distance there as well if youwant it to do it more often.
(;-) TP
-
I tried changing the value here but it makes no difference. It that the wrong value to change?
(http://img577.imageshack.us/img577/661/unled1vu.jpg)
-
Okay I figured it out, I changed the value here and that worked.
(http://img846.imageshack.us/img846/3209/unled2wb.jpg)
Now to figure out the right reference value to change. I want it to reference every 2 inches or so.
-
Here is where you set it.
function OnInit()
post.SetCommentChars ("()", "[]") --make sure ( and ) characters do not appear in system text
post.Text (" (Filename: ", fileName, ")\n")
post.Text (" (Post processor: ", postName, ")\n")
post.Text (" (Date: ", date, ")\n")
if(scale == metric) then
post.Text (" G21 (Units: Metric)\n") --metric mode
else
post.Text (" G20 (Units: Inches)\n") --inch mode
end
post.Text (" G53 G90 G40\n F1\n S500\n")
dist = 9999999
refdistance = 500 * scale <<<<<<<<<<--------------------------------------------Set RefDistance here
switchoffset = 0 <<<<<<<<<<<------------------------------------------- Set switch offset here
bigarcs = 1 --stitch arc segments together
minArcSize = 0.05 --arcs smaller than this are converted to moves
end
(;-)TP
-
Alrighty. Its back up and running. What a nightmare. Again thanks so much for helping me through this.