bCNC touch Plate

Talk about all things CNC
Post Reply
cfunk30
Posts: 6
Joined: Fri Apr 01, 2016 4:24 pm

bCNC touch Plate

Post by cfunk30 » Wed May 18, 2016 3:06 pm

Hi All,

Could anyone explain to me how to use a Z touch plate with bCnc? I have the touchplate setup and when I do probe in bCNC it lowers and stops when it touches but I am lost from this point. I have seen other posts about then entering Gcode commands. Is this still necessary or can I just put values in bCNC somewhere? (thickness of the touchplate for instance).
Do I zero Z before I do the probe? Also when the bit touches the plate it just stops, how do I get it to go back up a little so I can remove the plate?
Not looking to do any auto leveling, just setting zero for the z axis.
Do I type -(thickness of plate) in the Wpos box after?

Thanks for any pointers.

Chris

WillAdams
Posts: 8542
Joined: Mon Apr 09, 2012 6:11 pm
Location: Pennsylvania --- south of the Turnpike, East of US-15
Contact:

Re: bCNC touch Plate

Post by WillAdams » Wed May 18, 2016 4:07 pm

It's my understanding that the new bCNC has a pane specifically for this.

The wiki page on it has the line: http://www.shapeoko.com/wiki/index.php/Touch_Plate

>Send Grbl a G43.1 command with that difference.

It links to: http://www.shapeoko.com/forum/viewtopic ... 440#p45411

Does that help?
Shapeoko 3XL #0006 w/ Carbide Compact Router w/0.125″ and ¼″ Carbide 3D precision collets
Nomad 883 Pro #596 (bamboo)

cfunk30
Posts: 6
Joined: Fri Apr 01, 2016 4:24 pm

Re: bCNC touch Plate

Post by cfunk30 » Wed May 18, 2016 4:59 pm

Thanks Will,

Yes it does help. I guess I am just lazy, the paper method seems a lot easier than typing in gcode commands.
I sound like one of my users. "you mean I have to click on that AND move my mouse, sheese that is too much work" :-)

I think my version of bcnc might be a little behind. (can't seem to find where the version number is) maybe i'll try upgrading and see if it is any difference.

Thanks
Chris

RoguePirin
Posts: 216
Joined: Wed Sep 02, 2015 3:22 pm
Location: Illinois, USA

Re: bCNC touch Plate

Post by RoguePirin » Wed May 18, 2016 5:07 pm

Another option, if using WCS, is to adjust your Z position by the thickness of your touch plate. See cvoinescu's post here:
cvoinescu wrote:One piece of advice: you want them connected the other way round, the metal plate (insulated from the work) to A5, and the tool to ground. This is so that you collect the minimum of interference and reduce the chance of ESD destroying your Adruino.

So, measure the thickness of your touchplate. Say it's 3.33 mm. Place the touchplate on the surface you want to be Z = 0. Jog the machine to be a little above the touchplate, say 5 mm.

G91 ( incremental distance mode )
G38.2 Z-10 ( straight probe, 10 mm down )
G90 ( back to absolute distance mode )
G10 L20 P1 Z3.33 ( set G54 Z offset so that current position is 3.33 )

That sets the top of the touchplate to Z = 3.33, that is, the bottom of the touchplate to Z = 0, in the G54 work coordinate system (the default one). Replace P1 with P2, P3 etc. to set G55, G56 etc. Alternately, you can do G92 Z3.33, which will set the non-persistent G92 offset instead.
Shapeoko 3 #677, Nyloc nuts, ¾" HDPE base with t-nuts, Dewalt 611 w/Super PIDv2

ijv
Posts: 71
Joined: Sun Apr 06, 2014 10:41 am

Re: bCNC touch Plate

Post by ijv » Thu May 19, 2016 5:41 am

I don't have bCNC in front of me, but after the probing cycle you can enter the thickness of the touch plate in the "Z" WCS text box which is on the same pane as the probe command. This will give you a Z zero at the bottom of the touch plate, you can zero the X & Y WCS coordinates the same way. I'm pretty sure that bCNC just sends the G10 command that RoguePirin quoted.

Auarhau
Posts: 243
Joined: Tue Feb 25, 2014 8:46 pm

Re: bCNC touch Plate

Post by Auarhau » Fri May 20, 2016 2:18 pm

Been a while since I played with touchplates. But I also had some issues with the way bcnc solved it. I got used to the one in chillipepper and after that the bcnc one seems unfinished somehow.

In chilipeppr I believe you just enter the thickness of your plate and hit go. Then the software lowers the bit untill contact and then immediately sets 0 to the probe height - thickness of touch probe. And also moves the end mill up to a predefined Z location some X mm above the probed Z zero. Should be easy to make this happen if you can program:=) Which I dont...! :lol:
ShapeOko 2. Nema 17 74 oz·in. GAUPS shield on Arduino Uno. DRV8825 Drivers x4 . Kress 1050 FME-1. Z Acme Screw. Threaded inserts table.

vasilis
Posts: 22
Joined: Tue May 26, 2015 7:45 am

Re: bCNC touch Plate

Post by vasilis » Sat May 21, 2016 12:31 pm

In bCNC you can set the plate thickness in the TLO before probing and once it touches you can click on the Z=0.
If you want to have the same behavior as in Chillipepper you can set the gcode commands to be executed
directly in any of the programmable buttons. No programming is required at all.

cfunk30
Posts: 6
Joined: Fri Apr 01, 2016 4:24 pm

Re: bCNC touch Plate

Post by cfunk30 » Tue May 24, 2016 9:05 pm

Thanks All,

Makes much more sense now.

Quick question, where are the programmable buttons, or how do I add them? Can't seem to find any info on that.

Chris

vasilis
Posts: 22
Joined: Tue May 26, 2015 7:45 am

Re: bCNC touch Plate

Post by vasilis » Wed May 25, 2016 6:00 am

On the "Control" tab there are 6 red buttons with a label "User". If you right click any of the buttons
you can change the label, icon and the commands to be send, either g-code or bCNC commands.

Note that everything in bCNC is user configurable, (from the ini file) for example if you want
to have the "User" buttons on other tabs you need to add them in the ~/.bCNC file

cfunk30
Posts: 6
Joined: Fri Apr 01, 2016 4:24 pm

Re: bCNC touch Plate

Post by cfunk30 » Thu May 26, 2016 3:35 pm

Thank you all for the help.

Have it working like i envisioned it.

Used one of the programmable buttons.
Go to my G54 position
Plug my touch plate in.
Click the programmed button
Z lowers to the touch plate and then raises 10 mm
unplug touch plate, turn router on and run.

Here are the Gcode commands I ended up using in the macro

G38.2 Z-25 F100;
G92 Z20;
G91 G0 Z10.0;

Thanks again.

Chris

Post Reply