Router Forums banner
1 - 14 of 14 Posts

·
Registered
Joined
·
3 Posts
Discussion Starter · #1 ·
Hello all,

I'm having the hardest time determining the correct feed/speed even with all of the available calculators. I'm using VCarve Desktop 11 with a Bobs CNC Evo 4 and cutting into a solid piece of oak. (I switched from pine because of chipping and had some success with harder woods in a previous project.) I'm using a 1/4" 4-flute end mill (more on that in a sec).

I can't tell if I'm just at way too high of an RPM (and/or too slow of a speed) and therefore it's not "biting" and more or less just pushing into the material, but I'm aiming for the general area of the chip load as determined by various calculators. I found an excel sheet from a guy with a professional shop and for a 1/4" bit in hardwood it's suggesting 0.009-0.11 chip load. The bit sounded like it wasn't cutting properly and then in both attempts got caught or otherwise had a problem and sort of exploded the material in a small section. I was running about 17K RPMs with 600mm/min which VCarve tells me is a chipload of 0.0088, so right about what the other excel says.

Note: One thing that confuses me is that when I swap between mm/min and inch/min I'm getting much different chip load factors in VCarve. I was thinking that when I swap the measurement it would do a simply a conversion but it appears that it is simply saving the last value and I have to manually adjust? That, or is there some sort of difference between how chip load is measured between metric and standard? The difference is huge (600mm/min = 0.0088 but shows 0.0003 when I select inch/min) if I don't change any settings.

Wood Flooring Safety glove Floor Wood stain


Frustrated, I found a program written by BobCNC himself which helps identify the proper settings, however it says that using anything higher than 2 flutes isn't recommended because the router speeds are too high. I think this is likely my problem so I have a new 2-flute 1/4" endmill arriving Friday.

I'm also curious how to cut softer woods because of the chipping problem. I'd think a bit with less flute would actually contribute to that as it would be trying to cut out larger chunks at a time versus a faster/small bite.

Wood Organism Gesture Beige Font


As the username implies--very new to this! I'm sure I'm doing loads wrong so appreciate any help.
 

·
Administrator
David - Machinist in wood
Joined
·
4,361 Posts
Welcome to the forum! That looks like an upcut bit and that's why you're getting splintering. Use a downcut bit for that type of cut. I don't use metric but converting 600 mm/min get me to about 24 ipm and that's extremely slow for a feed rate with a 1/4" bit. I cut around 175 ipm to 250 ipm with bits like that for comparison (would be around 4445 mm/min to 6350 mm/min).
 

·
Registered
Joined
·
3 Posts
Discussion Starter · #3 ·
I didn't even think of the cut direction as I figured you'd want to clear out the residue to avoid problems... interesting. Is there ever any instance in which you'd want up vs down? I'm pretty much always doing this type of work (cutting plaque for someone) and other designs.
 

·
Administrator
David - Machinist in wood
Joined
·
4,361 Posts
Is there ever any instance in which you'd want up vs down?
Certainly. What I sometimes do is cut part way with a downcut bit and then switch to upcut or just use a compression bit. I probably use a compression bit more than anything else, it just depends on whether I'm cutting all the way through or part of the way through the work piece.
 

·
Official Greeter
Joined
·
20,101 Posts
G'day @CNCNewb , welcome to the forum.
 
  • Like
Reactions: CNCNewb

·
Registered
Joined
·
239 Posts
Don't know if this will help but I use a 0.25" 2 flute end mill at 15k rpm. I haven't tried oak. So far I get good results with walnut, maple, cherry, box elder and cedar. I haven't tried oak. But I don't like pine or hickory.
 

·
Registered
Joined
·
3 Posts
Discussion Starter · #8 ·
What about the fact that the app from BobCNC is saying the router is too high of a speed even for a 2 flute? Do you all have good results at router speeds with 2 or higher?

Rectangle Font Parallel Screenshot Number
 

·
Registered
Joined
·
86 Posts
I run in maple, African Mahogony, to cedar etc.. I use a downtown jenny 1/4" down- cut end mill from Cadence Manufacturing. It always cuts as smooth butter and I use it every day. Greatest, smoothest cut all the time. Last week I did this little piece in Ambrosa maple for a friend, his wife pasted. I pocketed out the pocket for the 3x5 picture, and the plastic, with a snap in fit, perfectly smooth, no sanding. They have a discount code if you ask for it too. When I carve with an end mill, the downtown jenny is my go-to every time.

Ray
Wood Font Rectangle Hardwood Landscape
 

·
Registered
Joined
·
106 Posts
4 flutes is twice the amount of flutes recommended. Stick with 2 flutes and the vetric feeds and speeds that come in the database for generic tools works great. Always keep in mind the size of the bit determines your depth of cut. 1/8" bit can cut 1/8" deep in one pass. 1/4" bit can cut 1/4" deep in one pass. I use a lot of red oak and it works good here.
 

·
Registered
Joined
·
1,605 Posts
Looks like a dull bit to me. You will get a lot more chip out if it is tearing rather than slicing.

Feeds and Speeds can be pretty mystifying. Start with the bit manufacturer - do they have recommendations for F&S and chip load? You can calculate the chip load if they have F&S. VCarve will do it for you. DOC is probably part of your issue. Bob's is a plywood machine - it will have some flex so you will want to run with shallower DOCs. Most manufacturers recommend a full diameter for the DOC but that is for an industrial machine with a fair amount of rigidity. I would start with 1/4 the bit diameters (for example, with a 1/4" bit - use a 1/16" pass depth) and work up from there. When you cut too deep for your machine, you will probably get chattering which promotes chip out like you are seeing.

Your 4 flute bit will have too small a chip load but that is probably not the cause of all that chip out. Too small a CL will give you dust rather than chips and maybe burning. A 0.0056" chip load is actually not unreasonable in hardwood.

When you change the units in vcarve, expect the CL to change because it is the thickness of a chip that is sliced off by the cutter and thus reported in units (mm or in)

See my blog on F&S for more info on F&S.
 

·
Registered
Joined
·
20 Posts
Looks like a dull bit to me. You will get a lot more chip out if it is tearing rather than slicing.

Feeds and Speeds can be pretty mystifying. Start with the bit manufacturer - do they have recommendations for F&S and chip load? You can calculate the chip load if they have F&S. VCarve will do it for you. DOC is probably part of your issue. Bob's is a plywood machine - it will have some flex so you will want to run with shallower DOCs. Most manufacturers recommend a full diameter for the DOC but that is for an industrial machine with a fair amount of rigidity. I would start with 1/4 the bit diameters (for example, with a 1/4" bit - use a 1/16" pass depth) and work up from there. When you cut too deep for your machine, you will probably get chattering which promotes chip out like you are seeing.

Your 4 flute bit will have too small a chip load but that is probably not the cause of all that chip out. Too small a CL will give you dust rather than chips and maybe burning. A 0.0056" chip load is actually not unreasonable in hardwood.

When you change the units in vcarve, expect the CL to change because it is the thickness of a chip that is sliced off by the cutter and thus reported in units (mm or in)

See my blog on F&S for more info on F&S.
I suspect that 4 flute bit might be made for metal, not wood.
 
1 - 14 of 14 Posts
Top