Hi, I am confused and as I am newbie I am sure it is an easy question for you folks. I am willing to my first job which is drilling my spoilboard. I did the job in Fusion and post process it with the recommended GRBL post processor but I am confused with the setting of Z. For X, Y my machine would be at its home position which is the 0,0 of my board in Fusion, sounds good. For Z, I am confusing. I thought I need to put the spindle bit touching the board (I don't have yet a Z probe) and "setzero" at this height in Control. But then I look into the GCode generated and in the GRBL post processor wiki, it is written: G53 G0 Z-2 Then at the beginning of each operation we move the Z-Axis (Spindle) all the way UP to its machine top - 2 mm. This is done to ensure that when we don't hit anything when moving to the starting position of the operation. We move UP to top - 2 mm io of just top, because on some machines moving up to top ( Z = 0) may trigger the limit switch. The G53 in the command makes this move in machine coordinates, instead of work coordinates. Going -2 will go down isn't it? and so do the opposite of what it is supposed to do and it will crash into the board. Or I should not "setzero" at the board level? (Note that this line seems to not be interpreted in the simulator of Control nor in ncviewer.com so I cannot check...) thx
you are correct, you 'setzero' at the surface of the board. the machine has 7 coordinate systems. the machine coordinate system (MCS) accessed by G53 the work coordinate systems (WCS) (6 of them, G54 to G59, default is G54) When you 'setzero' you are setting the Z zero for the current WCS which is G54 by default. When the machine homes it is setting the Machine coordinate zeros, and Z must be at its highest point, the positive end of the Z travel. Now, your text said G54 to G59 are modal, this means they stay set until changed, so you will see a G54 at the beginning of the Gcode and it stays set. G53 is NOT modal, to use it you have to give it one every line that needs it. so the command is G53 G0 Z-2 which means G53 = use machine coordinates G0 use rapid motion Z-2 go to the Z-2 position (in machine coordinates, which is the top of Z less 2 mm) if you have homed correctly at the top of Z then this command tells it to move UP to the top of Z less 2mm so it does not trigger the home switch which would cause it to stop with an alarm. now with the tool as high as it will go, the machine can move to work X0 Y0 safely without hitting anything (well, unless your table has as much junk as mine on it, in which case you need to be careful where you start a program (-: ) once the machine moves to the position of the first hole it will issue a command like G1 Z-3 F300 which means (note no G53 or G54 here, the G54 is implied) G1 move at cutting speed Z-3 go to WCS Z-3 F300 use feedrate of 300mm per minute
So the Machine Coordinate System is not visible neither editable? In OpenBuilds Control, I just see the WCS?
Correct - the machine co-ordinate system is literally a definition of the size of your machine. All work is done in a work co-ordinate system. Grbl remembers where you set the WCS zero in relation to the machine co-ordinate system so (unless you have a crash which might knock things out of line) WCS zero is a certain distance from machine co-ordinates zero - until you re-set it. Alex.
One more question for the same topic: setting Z0 I thought it would more precise, less risky etc to make the bit touch the surface of the board manually (=motor off, turning the Nema slowing by hand). But if I do this, I guess the MCS is then false (lose some steps that it doesn't see). So I guess it is not the recommended way of doing it... do you confirm it? (note : I do not have Z probe)
this is not a good way of doing it (research 'fake the home' for why, you do not want a false MCS nor WCS). machinists have been doing 'the paper method' since machines were invented, no need for fancy probes at all. I use as post-it note and have measured it as 0.1mm thick. jog Z to about 1mm above the stock change jog step to 0.1mm hold paper under bit and keep it moving. jog Z down till the paper catches. remove paper go down one more jog step (if you really feel the need) setzeroZ jog UP carefully (-: 0.1 is close enough for most things but you can spend the time to jog at 0.01mm if you want to. I have had power outs in the middle of many jobs, or had to hit e-stop, and having a reliable fake home and properly set WCS has saved the job every time. I can be cutting again after power-on in about a minute (-:
Ok interesting I just did my first job and do it the following way: - put the bit in the spindle but without tighting it (due to gravity, bit is well touching the board...obviously the spindle should not be to high) - put down the spindle at about the height where the bit is well situated into the spindle (the bit is still touching the board) - tight the bit in the spindle (bit is still touching the board) sounds good to me, what's your opinion?
You should not put the bit in the router too deep, it could bottom out and not be able to tighten properly. Put in all the way then pull back so about 1/4 of the shank is showing then tighten. If its in too deep and bottoms out the bit may not run true (wobble, make bigger hole) I use the metal duct tape (aluminum?) mines about .06mm thick, stick it on your project in a corner and hook up a set of aligator clips to your controller board and use the probe function (works great, just set under advanced functions .06mm) then probe.
My bit was not deep, just at the right level (there was a mark on the bit) duct tape is interesting solution!
I use the loose endmill in the collet method for zeroing on the spoilboard alot. It is a simple way to do it Here is a quick video of the aluminum tape method. I use it to find the center of circular stock so I can set my xyz zero in the middle.
One more question... Let's imagine I am milling 18mm wood theorically...but then once arrived in front of the machine, my wood is 18.2mm thick. I am not going back to the whole design to change from 18mm to 18.2mm but on the other side, I want to make sure the bit goes through the wood. My idea was to go onto the surface of the wood and then instead of doing that this reference is Z=0 (aka setzero), I would like to tell him that it is z=0.2mm, is it something doable with Control and if not how do you deal with it?
I run into this on most projects. When i get to my final cut out for my cribbage boards after all carving and drilling is done, I measure the final thickness of the board while its still mounted on the bed with a digital calliper and set this amount plus a couple of thousands to cut through, with tabs enabled so it doesnt fly around. ( measure all around my piece to get my average thickness, about four places, To get away from parallax errors) works for me.)
Forgot to mention, I’m doing this in Aspire, the program that I designed the board in, I just leave the last cut out depth, till I need it. Ste my values and save as gcode, then Control does the rest. I suppose you could rezero as before and Lie about your base height in the probe function to get the same results. Sorry if I confused the main issue.
Ok so in that case, I have to also make the 0 coordinate system in Fusion 360 in the spoilboard I guess to make it work? Indeed, sounds to me that it should work
then you also need to set your stock thickness to the largest you will ever encounter. if you dont the first cut may be much deeper than the machine can handle
I can try... So If I want to - Run some 18mm stock that may be 17mm, or 19mm, depends where you measure (; (If it really is 18.2mm throughout the whole sheet, I am saying you measured wrong hehe) - Want to cut through it without having stock remaining holding parts in place Then I would approach it in couple different ways: 1) The "not quite so deep first pass" - Surface the spoilboard - Zero endmill on the Spoilboard - Jog up say 20mm. Set Zero (So you know its exactly 20mm down till you hit the spoilboard) - CAM up as 20mm total depth of cut. Say 10x 2mm passes. - Become a clamping Guru, clamping stock so it doesn't bow, have no high/low spots, etc is harder than it sounds... - Run it - first pass will be hit (high spots) and miss (low spots) 2) The "Lets use the spoilboard for what it is" (The recommended way) - Zero endmill on top of the stock - CAM the job up as if its 20mm for arguments sake (more than the highest spot) - Run the job... The last pass will cut into the spoilboard but thats EXACTLY why its called a Spoilboard and not "forever-intact-board" - plus $20 every couple months is not going to kill you, and its soooo much easier 3) Precision jobs Not so much for 2.5D jobs, but if the part I am making depends on an exact height, exact pocket depths, and exact distance from bottom of pocket / shoulders, etc to backside of parts, then - Probe to spoilboard - Surface stock on an exact height - CAM up exact height (But I would never use this on a large area, or for jobs thats just through cuts mostly)
CAM the job up as if its 20mm for arguments sake (more than the highest spot) Is there an easy way to do that? or I have to go back in Fusion and change all the pieces from 18mm to 20mm?
Correct, setup the job as if the stock is 20mm thick knowing in your head that it will do some light/air cuts on the pieces that is actually lower. Lying to the CAM is always a useful trick
