I have the shapeoko pro XXL and i recently have been asked by a colleague to make some hardwood trays for him for his business. I will be cutting walnut, cherry, and hickory. My main problem is when using a 1/4" downcut endmill and the standard settings for hardwood it takes forever to even cut a 6"X6" pocket at 1/2" depth. Are there bigger bits I can use to speed up this process or can the parameters be adjusted at all? I am not sure what this thing is capable of so hardwood kind of scares me. Thanks for any help
Carbide Create library settings are meant to be conservative. You can experiment the following to increase material removal rate:
switch to an upcut endmill. downcut endmills are intrinsically limited to how far you can push them, because they tend to pack chips at the bottom of the cut.
increase depth per pass. For hardwood CC has a 0.04" per pass recommendation, but (especially on a Pro) you can pull off using deeper cuts. Anything below 50% of the endmill diameter is reasonable, for on that 1/4" endmill you may want to try doubling the depth per pass at 0.08". This will of course halve your cutting time by two.
increase feedrate and RPM by the same ratio. This will improve cutting while not changing the chipload. For example, CC recommends using 60ipm at 18000RPM. You can for example use 24000RPM instead and therefore bump feedrate up to 60 * 24000/18000 = 80ipm.
if the machine does not complain yet at that point, you can use the feedrate override button during a cut to experiment with slightly/incrementally increasing the feedrate. The machine will tell you when it can’t take it anymore.
To use aggressive material removal rate like this, you will however need to have very good workholding. Also, when using an aggressive toolpath to clear most of the material, you like likely want to use a finishing pass (that time the downcut endmill would be perfect) to remove the last 0.01" of material, to get a better finish.
The key is experimenting, because no two machines/workholding setups/material/endmill combinations are exactly the same.
As a general rule when trying to push your material removal rate (MRR) on these machines you will want to do the following:
Use the largest diameter tool feasible.
Maximize your width of cut before increasing your depth of cut. I typically do 75% of tool diameter before increasing depth.
As @Julien says, increase your RPM and IPM while keeping a reasonable chipload and not introducing problems that come from moving to fast such as skipping steps or extreme tool marks when the machine changes direction.
After all those things, increase your depth of cut until the machine starts complaining, then back off that point a little to give yourself a little safety factor.
This is interesting. May be Carbide3D could post better tools libraries for the Pro and HDM owners so that we can fully use our machines to their capacity (and save time ).
I know I could go edit all the csv file and adjust all the data but this would add the potential for mistakes.
Another option would be for CC to do it on the fly depending on the machine selected.
In all case, thanks for the info Julien.
Regards,
Rodolphe.
).