I’ve got a small project to make a router template out of 3/4" MDF for a friend and had planned to use a 1/4" spiral bit to cut it, but he needs a 1/4" hole in the center and I think in the past I’ve seen that the bit needs to be smaller than the hole.
Does anyone know if it is possible to do more of a drill than a mill operation on the X-Carve? I designed this in Fusion 360, but could fall back to Easel if necessary.
I couldn’t see why you wouldn’t be able to do this, especially in Fusion. I think it has a drilling operation, which is what you would want to use.
Does GRBL and the gcode sending function of Easel support the drilling operation?
On the GRBL wiki is mentions:
basic CAM features (profiling, pocketing, drilling)
so yes? Only one way to find out! Make sure you use the correct post processor!
I’ll have to try it. I use Easel for gcode sending and it seems pretty specific about which codes it supports.
GRBL or Easel’s gcode sending has little do with the drilling operations.
That is generated and performed by your CAM software (aka Fusion 360).
If you create a drilling operation inside Fusion 360, the X-Carve (aka GRBL) will obey it just fine.
The same principle can be applied to almost any CAM operation.
When I looked at the source code for Easel Local a while back it looked like it had a list of specific gcodes it was willing to send, and in fact that list seems to be downloaded on the fly from Inventables server, so it appeared that could be an issue. I didn’t get far enough to capture the list of supported gcodes and whether drilling was on the list.
But I could just be totally wrong.
Don’t overthink it.
- Easel will not allow you import an unsupported GCODE operation/
- Fusion 360’s post processor for Easel should only generate supported GCODE operations as well
- Fusion 360 will generate the code necessary to make due with the supported GCODE operations available.
So for example, if a drill operation gcode (which i don’t even think a specific gcode operation exists - OK they DO) doesn’t, it will use simply feed and move operations instead to peck and drill.
Update: OK they do exist (aka G81, G82, G83)
I’m a programmer, so overthinking things is an occupational hazard. Thanks for the info, I’ll just try it and see what happens.
Yup, it worked fine. I used the Deep Drilling - Full Retract option in passes. I did notice a fair amount of flex when it was drilling, the router was lifted up by the bit. I’ve got the bolts between the X Makerslides to stiff that, but I’m going to have to work on flex on the Y rails.
Umm. I don’t use easel, but doesn’t it have a manual mode?
Move the bit to the right location and then manually index the z axis into the work. You should be able to index it in and out several times to ‘drill’ the hole. If it fits (if you’re using a ¼" collet), manually drill the hole, but use a drill bit instead of the end mill.
The problems w/ drilling w/ an endmill:
- an endmill is four times better at cutting horizontally than a drill bit — conversely it’s only 1/4th as good at drilling/plunging
- any sort of deflection will result in a distorted hole — have to get plunge rate and depth of cut correct
- the size of the hole will be endmill diameter plus runout x2
- need to clear chips by “pecking” — moving the endmill in for the cut, then up and out to clear chips, possibly higher to allow vacuum to work, then repeating
Some CAM tools have support for drilling — MakerCAM is one free option which supports this. Grbl doesn’t support some of the specialized drilling G-codes, but one can use such G-code files by running them through a pre-processor which will convert such commands to more procedural ones which it does support.
The toolmakers trick is t use a 1/4" diameter silver steel rod and make it into a “D” bit. It will cut an exact 1/4" diameter. Plunge as you would a drill. Google search “D bit” for all the technical info.
CamBam shows the drill depth but Grbl ignores and fails to perform the drilling operation?? Any ideas.?
Is the drilling GCODE supported by GRBL?
Did you look it up?
I used MakerCam and UGS to make a cribbage board and had no problems with the drill operation
I/4 hole from a quarter bit. When I worked in the modeling shop we use to stick a small piece of tape on the bit so it was ecentric. It did fine most of the time.
GCode is move-to-XYZ coordinate commands, generally speaking. There may be a short form for a drill command, but the basic GCode commands should do just fine. If Easel doesn’t have a way of pocketing with the correct bit, you could always tell it you have a 0.2499" bit, couldn’t you? (I’ve never used Easel, so I’m not sure if it supports this, but I’ve used this trick in other software that didn’t support this feature)
I got my answer quite a while back when I found that Fusion 360 will generate g-code that the X-Carve can handle when you set up a drill operation. I did notice that the holes come out a bit oval due to flex during the plunge motion - the oval shape seems to be parallel to the Y axis. I’ve already got the wide Makerslide for my X axis so I’m wondering if it’s flex along the Y axis and I’m thinking about adding some reinforcement there.