Any advice on doing 2 bit carves? I am using a lowrider2 and want to do a double stack text sign using a 1/4 down cut bit for the roughing then switch to a 60 deg for some detail around the text. Any advice on keeping it all aligned and keeping the same depth when setting the z zero with both bits.
If you don’t have endstops this is tricky, because doing the bit change without moving the gantry can be tricky. If you have expensive material, the bit change is terrible.
I would probably use registration holes.
Put a piece of (prefferably inexpensive) material outside of the cut zone and with your roughing pass, drill down into it a few mm. Ideally, do this in 2 places separated on the X plane, so that you can check that you have the same square reference in both cuts.
I have been separating multiple bit cuts into separate job files for flexibility.
So your first job would have gcode something like:
G0 X-25.000 Y0.000 F2100 G0 Z0.250 F90 G1 Z-3.000 F30 G0 Z3.000 F90 G0 X0.000 Y0.000 F2100 ....
Then you would place the V-carve bit into the registration hole cut by the first job and issue
G92 X-25.000 Y0.000
to set the X/Y coordinates of the registration hole.
Of course you could substitute X0.000 Y-25.000 (Or any other value outside of the cut area too, if you choose.)
Both jobs would require you to zero the bit Z axis using the touch probe. If you zero to the same reference point, it should remain accurate. I would recommend that you do so to the same piece of stock that you drill your registration hole, so that it doesn’t get affected by any surfacing or the rough cut pass.
I’m just going to cut in pine until I get the hang of it. I have a z probe that I have never used so maybe try to get that going first.
I’ve been able to line up the two jobs (rough and carve) by making sure the gantry is cornered before starting, setting that as X0 Y0 initially (which it does when turning the machine on).
Then I travel the bit to where I want X0 Y0 for the carve, recording what that X and Y move is, then send G92 X0 Y0. Do the rough, bring the gantry back to the corner, change the bit and repeat the travel move I recorded earlier and repeat the G92 X0 Y0. It’s been really accurate. Kudos to the Lowrider design for that.
Usually I mark my zero on the piece to visually confirm I’ve returned to the correct X0 Y0. Using an external sacrificial piece for reference and registration holes like @SupraGuy suggests would make the visual check a physical check. That’s a great idea.
For Z I choose a spot that is not getting carved out to set zero before each carve. Remember the X,Y coordinate for that one too.
It’s not big deal to change bits without moving the machine, just use two wrenches to open the chuck instead of the stop. Squeeze the two wrenches together with one hand like a pair of scissors. I have done this about 20 times and never knocked the lowrider out if place. After a few tries it’s no big deal
As long as the steppers don’t power down, you shouldn’t have to worry about xy. When i had my lowrider, I thought it was much easier to just unlock the router and remove it to change the endmill. Then proceed to the xy where you set the z on the first operation and set the z again.
Really not much to it, once you do it a couple times.
On the Lowrider with most routers it is easy, just pull the router out of the holder and change the bit. You do absolutely need to use a touch plate of some kind with Vbits.
I also agree you can’t really do tool changes without probing z in between (unless you have an auto tool change… and even then you still are probing each tool during setup). That said, there are many ways to probe.
For a normal tool change… that is a second operation using the same workpeice fixture and origin… using a fixed z probe plate is best to preserve accuracy across tool changes. This is usually just a conductive plate permanently mounted off to the side. Since it never moves wrt the gantry, it ‘perfectly’ preserves z zero as you go through different bits for roughing/finishing. Just be sure not to turn off the motors until the last operation is done.
If the operation has a change in workspace origin (like a second clamping fixture), you will have to use a probe plate or similar to relocate z zero… and maybe even x and y zero depending on the fixtures used. It is best to avoid having to do this, unless there is no other way to cut the part. With some creativity and a machinist vise though, you can flip/rotate parts and preserv xyz zero.
Now to figure out the touch plate that I have!!
It is simple on a MPCNC, I have not tried it on a lowrider. Might be hard to reach in? I need to look at that.
The hard part (for me at least) was getting the clamp on the bit, so I just used a magnetic pick up tool like this:
Lately I’ve just been manually lowering on to a piece of paper and when the paper doesn’t slide, I’m at Z +.1mm This is the same way I level the bed on one of my 3D printers and it’s quick and easy.
Yeah, it was definitely not fun on the Lowrider. I stuck a neodymium magnet in the little clamp that came with the tiny touch probe, and it stuck to the collet holder pretty well. Did the job, anyway. If I did it again, I’d use a stationary switch as the touchplate like I did on my primo. There are 2 or 3 examples around the forum. Once it’s measured to z=0, you’re good to go.
The magnet idea sounds nice. I have a gnarly alligator clip I use for probing, but it can sometimes be challenging to clip onto tiny stuff like pcb drill bits. Would be nice if the spindle had a conductive path in the collet with an external terminal lol.
So can someone dummy this down for me. I have the touch plate from the store on the website. I have it hooked up and attached to the bit and the plate is under the bit. My under standing is to run G28 Z to have the z axis lower to the plate. I run that and the z axis lifts up. So I unplug everything and tried reversing the plug into the Z min on the Rambo board and run the same commands and the z axis lifts up again. I even run g28 Z-10 and it still moves up. I have got to be missing something. I read the page on the assembly and software but but it is a foreign language to me. I am not using end stops. I can put in commands to move the machine and everything moves as it should. Not sure where to go from here to get the touch plate working so I can run my rough and detailed cuts.
G28 Z on the lowrider homes up
Edit: Dan explains it better
Is this a LowRider?
In which case, G28 Z will home the machine to the top of its travel in order to square the Z axis.
If it’s a Primo, then G28 Z should lower the Z axis.
First off, place the router at the near left hand side of the machine. Move the axes individually. Increasing X should move to your right. Increasing Y should move away from you. Increasing Z should raise the tool higher over the bed. If these are not the way it moves, then something is backwards. This is the way it should work regardless of Primo, LowRider, MP3DP, ZenXY (Though that has no “Z”).
Arrange the motor plugs so that this is the way it behaves. Do each axis individually.
To home the Primo, G28 Z should go down until the (grounded) tool touches the (endstop pin) touch plate.
To home the LowRider2, use
I would probably make a custom menu item that issues:
G38.2 Z-100 G92 Z0.5 // Touchplate thickness G0 Z5 // raise Z axis to 5mm
You can also put that code into a .gcode file on your SD card, and just run it from the LCD.
Yes it is a lowrider2. When I enter in the command
It comes up as an unknown command. I am using Repetier Host for processing.
Edit. I did get it to work however the G38.2 command disables my z axis steppers and drops the z axis.
The G38.2 command needs to be enabled in Marlin.
In the configuration_adv.h file:
/** * G38 Probe Target * * This option adds G38.2 and G38.3 (probe towards target) * and optionally G38.4 and G38.5 (probe away from target). * Set MULTIPLE_PROBING for G38 to probe more than once. */ #define G38_PROBE_TARGET #if ENABLED(G38_PROBE_TARGET) //#define G38_PROBE_AWAY // Include G38.4 and G38.5 to probe away from target #define G38_MINIMUM_MOVE 0.0275 // (mm) Minimum distance that will produce a move. #endif
This is straight from the zip file for the LR2 dual endstop firmware package.
That’s part of the confusion – he isn’t using endstops so probably isn’t using the endstop firmware.