The largest ER-16 collet is 3/8", so I get that we can technically get as large as we can fit in that, but I assume that isn’t really the full answer to my question.
I’m guessing bit size, spindle power and frame rigidity are all related, and ultimately determine together what the true top-end of a machine’s capabilities are.
So how big of a bit can the X-Carve Pro handle? Did Inventables use ER-16 collets because the machine wasn’t capable of handling half-inch shanked bits? Is that the next step up in machining?
@AdamCook1 I’m going to guess you shouldn’t go over 3/8" bits. I’m not even able to run the XCP at the recommended feed/speeds of 1/4" Amana bits without the x& Y axis slipping. I’d imagine you’re going to have the same problem on a 3/8 or larger bit
Actually the largest is 10mm. (unless you have a larger on custom machined, which is technically possible, but it probably wont last long)
The shaft size itself doesn’t necessarily determine the load of the bit.
You can load up a 1/4" shaft bit by reducing Spindle RPM. increasing Feed and Depth per pass enough to cause damage so I wouldn’t necessarily say the shaft size was selected as a result of limitations of the machine… maybe as a deterrent to reduce unintended mis-use by a new CNC owner, But If used properly, I’m sure the machine itself can run a larger shank bit… could you take advantage of that larger shank to apply a higher load than with a smaller bit, probably not, but this goes back to the prior sentence about the shaft itself not being the single factor that determines load applied.
As large as you can get in a 10mm shaft, with respect to appropriate cut parameters.
Most Likely No, But I’m not a representative of the company, so take that as you will.
In my opinion: No; the next step is a more rigid frame (specifically wasteboard supports), followed by direct drive ball screws (get rid of the belts from stepper to ball screw), followed by rack and pinion (even more rigid and accurate), Then a larger spindle would be in order which could properly support larger tooling and higher applied loads.
Thanks @SethCNC. Sounds like the XCP really is the middle ground between a hobby machine and an industrial CNC. Great for running a CNC business, but not built for the crazy DOC and speeds that you see on the $40k+ machines.
This is honestly fine with me. It’s right where I am. I’m just trying to make sure I use the machine for what it’s built for, and avoid anything beyond that. There are a lot of fancy bits out there, and it’s not always clear which ones are a good marriage with this machine.
@GregBuckwalter I haven’t experienced any slipping yet. It would be nice to know your material, bit and F&S so I can keep that in mind.
Using an Amana Spektra bits ¼” 2-Flute Flat Bottom
Operating RPM: 18,000 / Dept of Cut: 1xTool Diameter (1/4”)
2 Flute Flat Bottom with Wood IPM 215-290 Chip Load Per Tooth 0.006” – 0.008”
I’ve run test at 285 ipm, 255 ipm, and 180 ipm. I’ve had X & Y slippage in every case. Had Z-axis slip in the 180 ipm with 50 ipm plunge.
I’ve been testing with standard lumber pine. 2"x12"
Inventable’s Customer Support recommends
Hard Maple Solid Carbide router, 2 flute, downcut 1/4"
RPM:16000 Depth per pass: 0.25" Feed rate: 160 in/min Plunge rate: 48 in/min
At 180 ipm the rough cut seemed like it was good. However, the 180 ipm 50 ipm plunge ball nose slipped with X, Y & Z
@AdamCook1 What speed/Feeds do you run at?
@GregBuckwalter With the 2-flute 1/4" spiral bit that comes with the XCP (Onsrud something something ) in hard maple:
- 13889 rpm
- 250 ipm feed
- 20 ipm plunge
- 1x doc
- 10% step over (not as sure if this is where it should be for my cuts)
I’ve had fast, clean cuts with this set up. Never anything wrong except when it’s been my fault.
Something to consider is that unless you are approaching from an edge, then the initial cut is a 100% engaged slot, so although 10% stepover is assigned to any stepover after that slot, that initial slot is 100%… and for that reason I tend to leave the stepover at 40% and use a slower feed rate.
Think about this… Altering nothing else but feed rate, IF I increase stepover from 10% to 40% that’s a factor of 4, so I could Decrease the feed by 4 and still complete the job in the same amount of time…
& I’m definitely not saying that’s the solution, It’s somewhere in between. More like 35-40% stepover and a feed of about 100IPM.
Good suggestion. I’ll probably do that. I have been using ramping to keep the pressure off the bit when beginning my cuts, but you’re probably right about finding more of a middle ground between engagement and speed. I’m guessing higher speeds are probably less accurate and harder on the material.
Here’s the new setting I’m going to try, per @SethCNC suggestion. We’ll see how it goes. Since slippage isn’t an issue for me, the only reasons for me to do this are better accuracy and cleaner cuts. This is a third of the previous chip load.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.