I’ve got a problem with my X50 Journeyman. I want to make holes for 5 mm steel pins. To make sure I get the right fit I’ve made a design with multiple hole sizes, ranging from 4.8 to 5.11 mm. However, cutting them leaves me with holes 6 mm or larger.
I am a novice using Fusion 360, but I have successfully cut things with great accuracy before. I have however reset the machine recently and moved it onto a new table. Maybe some settings are off, even though I have followed Onefinity’s guides while resetting.
Are you using a drilling operation or pocket? If it’s a drilling operation, you may be seeing the results of run-out where the router’s spindle is just a touch wobbly so the holes aren’t cut concentrically.
If it’s a pocket, make sure you’re doing an inside cut with a bit that’s smaller than the hole size. If you’re using VCarve, use a spiral cut so it moves down into the pocket in an expanding circle.
Update: I have updated the machine to 1.4.1 now, tightened everything and the holes I get are still 0.5 mm too wide. A hole that’s supposed to be 5 mm is 5.5 mm.
Tape a trustworthy ruler down on your waste board with a v bit at zero. Tell the machine to move as far as possible and see if it lines up with the ruler.
Are you using finishing passes? It’s possible the bit is just deflecting if your cuts are too extreme. It’s probably not this, but can’t hurt to ask.
So see if this is what you intended.
The top hole is 4.80mm dia.
The second hole down is 4.90mm dia.
The third hole down is 4.96mm
The bottom hole is 5.0mm
That is what the nc code is programmed for so if that is what you intended, with a 3.175mm cutter, then what you did in Fusion is good. The only thing I might wonder about is the feedrate 1666mm/m ramping down is fine but I wonder if 5000mm/m on the final pass at the bottom might be too fast to hold the tolerance.
Other things to look to for on the machine/cutter side is actual dia. of cutter - i dont remember if you said you measured it. Can’t always go by what’s on the tin. And wobble of cutter in the spindle. If you don’t have a dial indicator to measure that you can use paper method against the side of something for each flute on the cutter.
Sometimes when holding a tight tolerance, I will cheat the CAM program (Estlcam) by specifying my 1/8" end mill is .130 so the program thinks the end mill is larger than it actually is. Then as I run the program, I will adjust the stated tool diameter until I get the results I want. This method has served me quite well on various projects. If it’s a round hole, then this method is used with circular interpolation. If it’s a drill operation and I’m wanting something more exact than what I think the end mill will produce (or I lack the nominal size end mill), I use an undersize drill & then redrill or ream the hole on the drill press.
This is of course something you want to do on a single tool program, and not a larger program with multiple tool changes for obvious reasons.
Another thing that I don’t think I’ve seen mentioned here is bit deflection. Especially with smaller diameter bits, or bits that extend long past the collet/holder this can be an issue.
To test you can set a few holes to Conventional cut and a few to Climb. I don’t recall the precise terminology in Fusion but I know that setting is there. If they come out measurably different with identical tool paths then your bit is deflecting.
I’m doing the same thing right now…building cabinets with 5mm shelf pin holes…here’s what worked for me… I used a 3/16" bit. I tried the drill program first and the pins were too tight… they’d go in but you really had to force them… so I tried a pocket operation with the same bit but increased the size from .1875 (3/16) to .19… perfect fit
Just a thought, which you probably already had and done. When you measure the actual tool diameter, do you put that diameter into the tool database?
I’ve had problems getting proper hole sizes until I went in and measured all my bits and put the actual diameters into the tool database. That for the most part solve my problems. Again. Just a thought.
Were you using Fusion? Would you care to show your f3d-file or screenshots of how you set the tool path up? I can of course change the hole size, but I shouldn’t have to. A hole that is designed to be 5 mm should not turn out being 6 mm instead when milled. It’s crazy.
I think I have done that yes. Anyway, the bit is slightly smaller than the 1/8" it should be, so the holes shouldn’t be bigger than expected due to size difference. But thanks, I will most definitely double check when I’m back in the workshop.
