I have created a drawing on Sketchup, added ops for cutting a pocket and a slot and generated a CNC file. I'm cutting 18mm MDF and I don't quite understand whats happening when I run it. For some reason the cutter goes to the start position of the through slot and plunges straight through the MDF and then attempts to cut the slot at the full depth. I've set everything correctly as far as I can see. Files attached.
I see no problems with your drawings or your code. If you read the Gcode it looks like this (i have added explanations for pertinent lines) Code: G90 G21 G49 G17 F500 G53 G00 Z0.0 ; raise Z to safe height, Z home which is Z+ end of travel, high up away from table where Z homes. G00 X0 Y0 ; move to work 0,0 M3 S20000 G00 Z48.0 ; move to work clearance, 18mm workpeice plus the 30mm 'safe travel Z' that you set (Pass: 1) ; this proves that you have selected multipass X58.45 Y105.6 ; start of cut G00 Z18.5 G01 Z17.0 F500 ; 17mm above zero when table is Zzero is 1mm down into the workpiece Y252.4 F2500 X61.55 Y105.6 X58.45 (Pass: 2) Z16.0 F500 ; now 16mm above table Y252.4 F2500 X61.55 Y105.6 X58.45 (Pass: 3) Z15.0 F500 ; 15mm above table, and so on. The other file is similar, no problems. Are you homing? If no home switches, then are you faking the home? Where are you setting the work zero? Your drawing specifies front left corner and 'table is Z zero' which means the bottom of your workpiece. The top of the workpiece is generally easier to probe or touchoff but there can be good reasons for using the table as Z zero.
Hi I move to the cutter manually to the bottom left corner and against the table top. I then press reset zero on UGS. I have never set a home position, should I?. This is the setup I have always used without previous problems. I can only assume there is a problem with the XPRO Controller. I'll look at that and the grbl settings in UGS. Thank you for your help.
Yes you should fake the home as per my previous link. That will not cause the symptoms you asked about so now I am somewhat confused.
It does, because where i had set the router motor the Z Axis reached the top before it could achieve 30mm above the workpiece. When it plunged into the MDF sheet it was then starting lower than I had set it. When I reset the safe height to 3mm it was fine. I will a). Invest in limit switches and b) set a fake home position. One more question for you. First time I've tried a counterbore and it keeps coming up saying the numbers I've input make no sense. I have 18mm MDF with a 6.3mm cutter. I need a 12mm dia through hole with a 20mm dia x 55mm deep counterbore. What would the settings be please.
ah! you did not mention that it crashed before cutting too deep! I assume you mean 20mm dia and 5.5mm deep not 55mm deep which generates Gcode like this (with 'depth first' option on). it will do the 12mm hole first then helical bore the counterbore in stages going outward (30% bit diameter in this case). with 'depth first' false it will do something like this, does the 12mm hole to depth first, then does the counterbore as a 'spiral out'. In this case multipass is off so it does that 5.5mm depth in one go, if multipass is on it will do multiple spiralouts as increasing depths. also, with multipass off the ramp angle is limited by the 'ramp in Z' angle, 5 degrees is shown. with multipass ON the ramp angle is limited to the lesser of multipass depth per turn and ramp angle. It is all in the manual.
