sheetcam.com

Posted: **Fri Jul 03, 2015 4:45 am**

Maybe i misunderstand the conceot, but drilling i always have problems with. I have these settings and always get rapid movements where they should be feed see

Cut depth set to 15mm
peck depth 5mm
Peck retract 2mm
Plunge rate 50mm/min

N0170 G01 Z-5.000 F50.0
N0180 G00 Z-8.0000
N0190 Z-4.0000
N0200 G01 Z-10.000
N0210 G00 Z-18.0000
N0220 Z-9.0000
N0230 G01 Z-15.000
N0240 G00 Z10.0000

I would have thought that the operation would have gone

set feed rate -5mm deep, retracted to-3mm at rapid, rapid back to -5mm and start drilling again at 50mm/min, to -10mm, then rapdi back to-8mm, rapid back to -10mm, drill at set feed to -15mm and be done. is there a setting i have wrong?
this is set um on a milling machine with mach3. Les can you help me figure this out.

Posted: **Tue Jul 07, 2015 5:14 am**

Can any1 help me figure this out is there a setting I have wrong?

Posted: **Tue Jul 07, 2015 3:29 pm**

That's an odd one. What post processor are you using? Could you post a job file demonstrating the fault.

Posted: **Tue Jul 07, 2015 3:59 pm**

In the simulation it always works perfect. only when it rights the code it does this every time. what do you mean by a post processor?
Sheetcam, Mach3 is all I use?

Posted: **Tue Jul 07, 2015 4:08 pm**

If you go to Options->machine->post processor you just have the Mach3 post selected? That post should be fine. Could you post the job file so I can run it here and try to figure out what is going on.

Posted: **Tue Jul 07, 2015 5:31 pm**

I'm not near the machine now, but from memory I have that selected, and Rotary Mill. Ill try and get you a job file within the next 24hrs

Posted: **Tue Jul 07, 2015 9:37 pm**

Post Processor is Mach3 Rotary (edited)

Mach3 4th axis rotary post processor

For milling/routing with the PlasmaRotary plugin

Posted: **Tue Jul 07, 2015 9:39 pm**

and the job file

Posted: **Wed Jul 08, 2015 1:19 pm**

This looks like a bug in the rotary helper. I'll fix it properly for the next release but you can fix your copy yourself. Run SheetCam as administrator (right-click on the SheetCam shortcut->run as administrator). Now go to Options->plugin options->RotaryPlasma and click on the 'edit macro' button. In the editor go to File->open and open the RotaryHelper file. In there replace function OnRapid() and function OnRapid2() with the versions below:

Code: Select all

function OnRapid&#40;&#41;
--post.Text&#40;"   R  ex = " .. endX .. " ey = " .. endY .. " ez = " .. endZ .. "\n"&#41;
   local tx = endX
   local ty = endY
   local tz = endZ
   if&#40;endX >= 1e17 or endY >= 1e17&#41; then return end
   sc.QueryDll&#40;qrySETXSTART, endX, dllId&#41;
   sc.QueryDll&#40;qrySETYSTART, endY, dllId&#41;
   sc.QueryDll&#40;qrySETZSTART, endZ, dllId&#41;
   if&#40;endZ >= safeZ&#41; then
      local z
      if&#40;endZ > 1e17&#41; then
         z = sc.QueryDll&#40;qryGETSAFEZ, 0, dllId&#41; + safeZ
         endZ = 0
      else
         if&#40;currentY > 1e17&#41; then
            z = sc.QueryDll&#40;qryCHKEND, endY, dllId&#41;
         else
            z = sc.QueryDll&#40;qryCHKEND, currentY, dllId&#41;
         end
      end
--      rotaryVals.z = z
      if&#40;z > rotaryVals.z and currentX < 1e17 and currentY < 1e17&#41; then
         endX = rotaryVals.cx
         endY = rotaryVals.cy
         endZ = z + endZ
         DoRapid&#40;&#41;
         endX = tx
         endY = ty
         endZ = tz
      end
      rotaryVals.z = z + endZ
   else
      sc.QueryDll&#40;qrySETZ, endZ, dllId&#41;
      rotaryVals.z = sc.QueryDll&#40;qryGETZ, 0, dllId&#41;
      if&#40;ignorePierceHeightMove and endZ < currentZ and endZ == pierceHeight&#41; then
         endX = tx
         endY = ty
         endZ = tz
         return
      end
   end
   OnRapid2&#40;&#41;
   endX = tx
   endY = ty
   endZ = tz
end

function OnRapid2&#40;&#41;
--post.Text&#40;"   R2  ex = " .. endX .. " ey = " .. endY .. " ez = " .. endZ .. "\n"&#41;
   currentX = rotaryVals.cx
   currentY = rotaryVals.cy
   currentZ = rotaryVals.cz
   endY = sc.QueryDll&#40;qryRAPIDY, endY, dllId&#41;
   endZ = rotaryVals.z-- + endZ --sc.QueryDll&#40;qryGETZ, 0, dllId&#41; + rotaryVals.z + endZ
   endA = sc.QueryDll&#40;qryGETA, 0, dllId&#41;
   DoRapid&#40;&#41;;
   rotaryVals.cx = endX
   rotaryVals.cy = endY
   rotaryVals.cz = endZ
end

Posted: **Wed Jul 08, 2015 1:37 pm**

N0170 G01 Z-5.000 F50.0
N0180 G00 Z-4.0000
N0190 G01 Z-10.000
N0200 G00 Z-9.0000
N0210 G01 Z-15.000
N0220 G00 Z10.0000

Fixed thanks heaps for that.

While i've got you how do i fix this? everything works fine just does this on start up.

Posted: **Wed Jul 08, 2015 4:17 pm**

I've never seen that before. It looks like your ini file has been damaged somehow. It won't do any harm but if you want to fix it go to Help->open settings folder. Send me a copy of the ini file and I'll clean it up for you.

Posted: **Wed Jul 08, 2015 10:50 pm**

Emailed it to you Les as it wouldnt attach for some reason

sheetcam.com

Peck Drilling issue,

Peck Drilling issue,