Peck Drilling issue,

Problems and questions
1

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.

2

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

3

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

4

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?

5

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.

6

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

7

Post Processor is Mach3 Rotary (edited)

Mach3 4th axis rotary post processor

For milling/routing with the PlasmaRotary plugin

8

and the job file

9

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:

function OnRapid()
--post.Text("   R  ex = " .. endX .. " ey = " .. endY .. " ez = " .. endZ .. "\n")
   local tx = endX
   local ty = endY
   local tz = endZ
   if(endX >= 1e17 or endY >= 1e17) then return end
   sc.QueryDll(qrySETXSTART, endX, dllId)
   sc.QueryDll(qrySETYSTART, endY, dllId)
   sc.QueryDll(qrySETZSTART, endZ, dllId)
   if(endZ >= safeZ) then
      local z
      if(endZ > 1e17) then
         z = sc.QueryDll(qryGETSAFEZ, 0, dllId) + safeZ
         endZ = 0
      else
         if(currentY > 1e17) then
            z = sc.QueryDll(qryCHKEND, endY, dllId)
         else
            z = sc.QueryDll(qryCHKEND, currentY, dllId)
         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
10

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.

11

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.

12

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