|
Post by James@fireaxe on Aug 20, 2018 11:57:16 GMT
If you use the same endmill and touch plate everytime you zero a workpiece the whole process could be written in G-code and automated. You could also use the circle of the touchplate to find the zero of the workpiece, but that's a bit more complicated. Typically I use a bigger end mill to start, like a 1/4 inch (or 1 inch face planer) then I use smaller ones there after. So when switching end miles, I'll need to do the XYZ touch plate zero?
|
|
|
Post by Bruce on Aug 20, 2018 19:03:12 GMT
Once the X and Y position is found and zeroed then all you need to do is zero the Z axis when you change each tool. The touch plate height above the work piece would be added to the z axis zero. e.g. if the touch plate is 5mm thick when the probe stops to the top of the plate +5mm is entered as the z axis zero. This assumes the touch plate is sitting flat on the work piece.
|
|
gisco
New Member
Posts: 15
|
Post by gisco on Aug 24, 2018 15:34:40 GMT
To berogers Can you use a flat aluminum plate hooked up to the sel & gnd to zero only the z axis
|
|
|
Post by Bruce on Aug 24, 2018 19:44:35 GMT
Yes, that should work. You can set the X and Y by sight and use the touch plate for the Z axis if you prefer.
|
|
|
Post by roybartels on Dec 4, 2018 23:37:37 GMT
If I connect the touch plate how to I go about using it. Do I need to write some g-code?
if I lower the bit (z axis) does it just stop when the bit touches the plate?
|
|
freik
Full Member
"What did you buy the new CNC Router for?" "To make stuff for my CNC Router!"
Posts: 107
Location: Bellevue, WA
Machine: Power Route
|
Post by freik on Dec 5, 2018 16:52:07 GMT
If I connect the touch plate how to I go about using it. Do I need to write some g-code? if I lower the bit (z axis) does it just stop when the bit touches the plate? UGS (I'm using platform 2.0, build from September 2018) has a "probe module" that automates everything. Enter the thickness of the touch plate, attach the probe, and away it goes. Very straight forward...
|
|
|
Post by roybartels on Dec 11, 2018 11:48:37 GMT
Thanks Freik. I attached the probe and am able to set z much quicker, probably more accurately too. Having a little trouble understanding the settings though. I would like it to set the G54 Z to the top of the material but it sets it approximately to the top of the plate. The plate thickness seems to have little effect. I'm working in inches Does the thickness needs to be in mm? I'll play with it more tonight.
|
|
|
Post by Derek the Admin on Dec 11, 2018 12:09:19 GMT
I personally don’t use the UGS probing functionality because I’ve found it to be finicky. I use commands like this (assume you are in inches and in absolute) G38.2 Z-5 F8 (probes downward towards Z-5 at a rate of 8 IPM After contact, to set the height for the G54 system: G10 L20 P1 Z0.79 (where Z0.79 is the probe thickness. Substitute your actual value here) Jog up, pull puck.
|
|
|
Post by James@fireaxe on Dec 11, 2018 12:18:27 GMT
Derek,
So by using your method, you are still able to probe without using the UGS probe function? Assuming wires hooked up and connected to the bit and plate.
Is this a stand alone .nc file created prior to loading the work process file?
So the procedure would be, jog machine to your work XYzero. Place puck. Load and run probe file. Your Z is now set. Load work file, hit play?
As you said, in the work process file add the following
"G10 L20 P1 Z0.79" (where Zxx is actual thickness. ) Does this line replace the G54 line?
Can you post an example of a probe G code file, and an example with the addition of the G10 line in a regular process file?
Thanks much
|
|
|
Post by Derek the Admin on Dec 11, 2018 12:49:46 GMT
Hey James. Those are just commands typed into the commandline. I don’t actually run probing in a file. The two commands that I listed are all I do to probe After I jog the machine to the desired probe position and attach the clip and position the puck under the end mill. That G10 command rewrites the Z value for G54. Typing G54 just selects the G54 system (Grbl and other controllers are in G54 by default by the way), but that G10 command is needed to change what’s stored in the control’s memory for where the G54 position is. Instead of using G10, you could use G92 Z(desired z value here). The only “problem” with that is G92 creates temporary offsets that are forgotten whenever you hit the stop button in UGS, your g code program sends an M30 (end of file command), or you power down the machine.
|
|
|
Post by James@fireaxe on Dec 11, 2018 13:10:07 GMT
So I wouldn't need to add anything to my .NC files after F360 writes them for this probing procedure?
Just run the commands as you state, then run my work piece files? And run each time a tool is changed?
|
|
|
Post by ttabbal on Dec 11, 2018 17:42:17 GMT
You don't need to change the work files. Just probe and save the new zero. Remember to include the height of your probe puck. The one that came with my Power Route is 20mm, so when I hit, I'm at Z20. So I would send:
G10 L20 P1 Z20
Then jog up so I can remove the puck and unclip the wire.
I'm using CNCjs, which does all that for me as part of the probe command and seems to work well so far. It actually moves up 4mm after the touch and sets to Z24, but both methods do the same thing. Now when your gcode calls for a 1mm cut, it goes 1mm below the surface as you would expect, so no need to modify the gcode. I've only done a couple tool changes so far, but the basic order is..
Set X/Y zero to match whatever location I wanted to use. Set the puck out, clip on, and probe. This sets Z0. Run the file.
When it's done with that one, turn off the router, swap tools. Set the puck out, clip on, and probe. This sets Z0 for the new tool. Run the next file.
If you are using an xyz plate, it might be a good idea to use a ground rod for the probe of X/Y. If you happen to hit inside a flute on the endmill it could throw off the location. Not much, but it's something to be aware of.
|
|