I get a strange step or kink at the start position of a carve. It’s only at the start position and does this on all the cut outs. As if the plunge location is slightly off from the cut
I’m using Aspire and UCGS and have tried gcode sender as well.
I’ve tried looking on the forums but haven’t found anything yet.
Can you post your g-code?
Could it be the bit deflecting during the initial plunge cut?
What is your Plunge rate?
The max a stock XC is rated at is 500mm/min (19.6 inch/min)
(Edit its mm/min not sec - oops!)
What kind of bit are you using? Spiral? (you want to make sure your bits are made to do plunge cutting. Most are but it is a good idea to be sure)
You might want to try the Ramp Plunge moves option. Depending on the cut operation you may have different choices.
I tend to use fixed angle or fixed distance and avoid spiral (constant ramping over the whole operation). As ramping slows the whole cut down to the plunge rate. and the greater the ramping the more time it adds.
(The first time I tried it I selected spiral and could not figure out why my 10 min cut was now well over a hour.)
And of course check your V Wheels and belts.
Here is the gcode for the circle:
G17
G21
G0 Z20.0000
G0 X0.0000 Y0.0000 S12000 M3
G0 X20.3571 Y9.2564 Z6.0000
G1 Z-2.0000 F300.0
G3 X32.8865 Y21.7857 I0.0000 J12.5293 F1800.0
G3 X20.3571 Y34.3150 I-12.5293 J0.0000
G3 X7.8278 Y21.7857 I0.0000 J-12.5293
G3 X20.3571 Y9.2564 I12.5293 J0.0000
G0 Z6.0000
G0 Z20.0000
G0 X0.0000 Y0.0000
M30
Ive checked my belts and vwheels but all seems fine.
It seems to be no matter where the the plunge point its off.
Ive dropped the plunge rate down to 200mm/sec
I think its a 2 flute straight bit.
im very new to the cnc arena so i might miss something thats obvious
This is a long shot but make sure the bottom of the bit has a sharp edge to it for plunge cutting.
I recommend going to the hardware store and picking up a 1/4" spiral upcut and a 1/4" spiral down cut bit.
The upcut will be your go to bit for most woods and the downcut for plywood and MDF.
(Unrelated tip I also recommend a Dust Deputy for your shop vac, it makes a HUGE difference with the fine dust that otherwise blows right through the vac. Especially if you are working with MDF)
The code looks good, the plunge is definitely in the correct spot and the speed seems fine (it’s 200mm per minute though!).
It’s most likely not a bit meant for plunge maneuvers. As suggested, try an upcut/downcut/compression cut bit.
Thanks for the tip. I’ll probably need to look around to see if they are available otherwise I’ll make one.
The bit does have a sharp section on the underside. But I’ll try see if I can get bits that fit.
Thanks for the help
just from the picture, I’m guessing there is some play on the z and the bit is grabbing and deflecting on the initial plunge
thanks Ill look to see if there is a problem there as well
make sure it is not a side cutting bit only otherwise the bit is going to wobble all over on the plunge.
Since you are using Aspire, take a look at ramping in and lead-in on a toolpath. So even if the bit does not cut well on a plunge, it can still work fine on a profile cut like you are doing.
Thanks everyone for the assistance. i tightened up my z axis where i could and i tried the ramp plunge option with the current bit I was using earlier and the circle no longer has that kink in it.
Time to invest in more bits seeing as the machine is behaving as it should.
Don’t be afraid to use the machine. It runs great once you get everything tuned. It sounds like your bit may have not been bottom cutting.
