So I thought I was doing pretty good seeing that I had about 10 or so successful projects done on my MPCNC. This was until I tried to cut out a US Flag union for buddy which has be basically perfect.
Here is my spoil board pocket area thats meant to be changeable once its cut up. I used particle board as my spoil board.
I used a 90 degree vbit with a 1/2 cutting dia. The wood was 10.5 x 14.75" and my MPCNC cutting area is 23 X 35".
Heres my first attempt…I didnt realize at the time but the wood was slightly cupped and actually had a small rock to it. Another rookie move was the wood was not fixtured perfectly straight.
You can see in the upper section the stars are much fatter than they should be. Also the lower row of star (which look right sizewise) are crooked.
I flip over the piece since its scrap now to test and shim out the wood so its not rocking anymore and also get the wood lined up straighter using the X axis and the bit riding near the edge. I decided to touch of Z in the middle vs the corner thinking maybe it will help look less obvious if there is some warpage.
You can see it looks better but the stars are still not all the same.
So now I start checking my corner piece heights and they are not exactly all the same height I cant recall the numbers but it was enough to raise concern. So id like to correct everything and get this beast as flat as possible. Let me know if these steps are correct?
First measure and set all feet to exact same height
Run a fly cut bit over the entire spoil board using a pocket program
Check machine with dial indicator somehow mounting it
Fly material if its really bad both sides
I most likely never noticed it being this far off because I haven’t ran anything with repeating patterns this big.
Carving is very strict on Z accuracy. There are some things you can do to make it less strict:
use a sharper bit. The error on a fat bit is going to be larger. Imagine cutting 1/8" too deep, a 90d bit will be 1/8" wider than it should be a 45d bit will be closer to 1/16"
break up the job, and set a new Z between parts. If you zero the Z for each star, you’ll get very good results. If you group them by 5 stars, or 10 stars, you can find a good balance. Just keep the machine alive between cuts. The only thing you’re changing is the Z height, so you can do G92 Z0 for each new file.
Surface the top of the workpiece first. It won’t be “flat” but it will be the same “Z height”. You could technically do it after as well.
The shape and curving of the stars has more to do with your speeds for that bit. A wide bit is hard to get right because the middle is moving so much slower than the edges. So take it slow. You can also do a finishing pass.
Makes sense bigger bit more noticeable. I was trying to save time with that big bit however may have hurt me more.
Interesting idea about breaking the job up and re zeroing it. So im trying to think about how to lay that out in the Gcode. So would I group a smaller section of stars create a toolpath and post it, after posting it just keep dumping those into a bigger g code file?
Or just stop it the entire thing periodically with a
M17 X,Y (to lock up steppers except z)
M0 (set my Z on the top of the part)
G92 Z0 (set zero)
I have a low rider, so if I let go of the Z, it would plunge. So I would do separate jobs. If you’re confortable with the M0 and M17, then go for it. Just make sure you don’t have an G92s in the middle.
Yeah my Z drops very little so maybe ill give that a shot. Would it be wise after the g92 was put into place to send it up so it doesn’t travel with the bit down? Actually crap where would be the best place for the M0??
M17 X,Y (to lock up steppers except z)
M0 (set my Z on the top of the part)
G92 Z0 (set zero)
G01 Z 10.0
You just have to think through how you want it. You might do the longest option:
G1 Z10 F300
G1 X<something> Y<something> F1200
M17 X Y Z
M0 Turn off spindle
M17 Z0
M0 Set new Z
G92 Z0
Maybe? You need to have the xy of where you want the next Z probe to start.
What I would do with my machine is just make files as though I was cutting 5 different jobs. In my start gcode, I don’t have G92 and my motors are configured to stay enabled forever. So after the first job, I would stop the spindle. Use the buttons to move the XY to a new place. Then lower Z to the right height. G92 Z0. Move the bit up 1cm or so. Start the spindle and then start the next gcode file.
I am saying make toolpaths for a couple of stars, save the gcode, delete the toolpaths, make a few more, save gcode, etc. Then just cut one, reset the Z, and cut the next one.
Yeah I put G92 x0 y0 z0 that in thinking I needed to
If I do the sections of stars like you said…what would happens to my home position and stop position after each round? I would need a G92 Z0 at the beginning of each cut right? Im sure im overthinking it.
Putting it in the file is the same as sending it before a job. The difference is, if you send G92 Z0 instead of putting it in the file, you can move the Z around after the G92.
It finally registered as to what you’re saying. I broke that project up to 6 different toolpaths. I didn’t even make past the 1st set of 5 stars though due to height variations. Clearly there’s some problems with this material. This was supposed to be a paying job. But there’s no way I want to sit there and set the z depth for 50 stars lol. I told the guy plane the wood or get better wood.
But the jist of it would be move the head to a center location of the star grouping, manually move the head just over the top of the part hit G92 Z0 in repetier. Raise head slightly and manually move to start point of project hit G92 X0 Y0 in repetier. Drives me nuts that repetier doesn’t change its xyz to zero thank god for the LCD. Hit the program go rinse repeat with each grouping being careful with my G92s.
Unfortunately this wood was pretty bad. Just to make sure I wasn’t crazy I ran the same test and a piece of oak that was much better. Better being more consistent repeated stars.
A planer can push hard enough to flatten out a board before cutting it. In general, if you have a thin cupped board, you need to use a joiner to flatten one side, then the planer to make the other side parallel. You can make a sled for the planer that will shim under the high spots on the board so it can’t smash the board down.
Ahhh yes I know old man has one of those in the corner…I wasn’t sure which would be better for flattening out cupped boards. Looks like the joiner might be better for my application vs planner.
Would it be best to just always run both sides using the joiner both sides then plane both sides? Just trying to figure out a process. Granted this process would reduce the overall thickness of both sides but I dont have like a thickness spec or anything.
Well, technically, if his joiner is well-tuned, and he has enough thickness, he can flatten one edge, then make both sides perpendicular to that edge… But that’s a theoretical edge-case and only valid when a planer or drum sander is unavailable.
