Cut depths and spindal speeds to improve finsh time

**Fivetide** · 19-02-2013

Hi guys, at the moment I'm a moderately complex carving out of light density hard wood ( mainly American Walnut) 200 x 200 mm to a depth of 17 mm. To complete this its taking nearly twelve hours. I use a 6 mm end bit to rough out the block then a 3mm ball nose to finish. I have however realised that I could actually get away with a 6 mm ball nose that I will buy from flea bay tonight. What I was was wondering is , is there a cutter / bit that can cut at that depth in one go ? And what in you opinion is the maximum feed rate for this material ? Have you any tips for speeding up production please ? And one more question, I'm having trouble when swapping the bits from rough to finish as in they have different shank lengths and therefore I cannot simply push it to the top and it will be at the correct depth in the chuck, anyone any tips on how to swap out bits so they are at the same depth or should I just buy end and ball nose bits with same length shanks to make things simple ?

**GEOFFREY** · 20-02-2013

You may not be able to get same length shanks, and even if you do you will still need to reference them to the same length. If you make a collar to fit the shank and lock it off at your Z 0, you can then do the same to ensure your other tool has the identical protrusion. I use a length setting press and all of my tools always are exactly the same length. I have to admit it is easier for me as I only use 3.175mm shanks. G.

**AdCNC** · 20-02-2013

Id say you could do it on one go with a good carbide 6mm Ball 2 flute, you would have to ramp/zigzag down on the entry to the Max Z Depth at the start then travis back and forward using a mix of climb and conventional milling with a 0.2mm Step over. All depends on spindle and machine rigidity.

**JAZZCNC** · 20-02-2013

While it's possible I wouldn't cut 17mm in one pass has it will impact on finish and stress for tool, also risk of tearing the material depending on grain.
Quick Z level roughing won't take long with 6mm straight flute cutter and 3mm step which will greatly improve finish and work load for ball-nose finish cutter.

Regards tool change then your way of using shank length is asking for trouble and very unreliable. Bottoming the shank out in the spindle is bad for the spindle and it's bearings transferring heat and shock loads straight into it.

Presume because your not working off the material surface to reference new tool that you have chopped it away.? . . . In this case then you may find it easier to position your model in Cad so all moves will be in the positive direction and the bottom is at Zero in Z axis. This then means you can reference all tools off the bed and so long has you set enough rapid clearance height in Cam to clear material height you won't have a problem.

Another and far easier way if you use Mach is to setup a touch plate probe and use a screen set like Gerrys 2010. The CNC Woodworker - Mach3 2010

This has great feature for changing tools were after first initial touching off top of material it keeps track of the tool offsets and by touching off a fixed probe point it AUTO sets the tool height offsets for you and all you do is change the tool. Doesn't matter how far shank into spindle or tool length it does all the calcs and setting zero's etc.
You can even tell it where on the machine you want it to move too for changing the actual tool before it goes off and finds the new tool height.
If set up to do so it will start the spindle and carry on thru the code or wait for you to start spindle then carry on.

This combination of Fixed and moving probe plates means you can either very quickly manually set Z height off any point or like in this case were 3D model gets top surface cut away makes tool changes very easy and very accurate with the full Auto tool change.
Another Plus and great asset when used correctly and in conjunction with movable probe plate is the other probe options for things like finding centres of holes or circles, corners of parts, edges of parts, parallel edges etc

**deebo** · 19-05-2015

Im having the same problem only Im cutting 25mm mdf. 110mm alphabet A to Z. Im using a 6mm spiral Leitz tool. Spindle speed set at 5000rpm and feed at 7000 although I have this slowed down to 40% as strain on tooling . Im cutting this in 2 steps but its taking over 2 hrs to cut 144 letters..boss thinks Im swinging the lead. If I speed the rpm and feed up it breaks the tool. Are my speeds correct?

**GEOFFREY** · 20-05-2015

Hi, No expert, but I cut 15mm ply and 15mm mdf at 6m/min and 18k rpm using either straight or spiral 2 flute cutters and break very few. I am of course aware that I will probably be told that I'm doing it all wrong!!! G.

**JAZZCNC** · 20-05-2015

Originally Posted by GEOFFREY

Hi, No expert, but I cut 15mm ply and 15mm mdf at 6m/min and 18k rpm using either straight or spiral 2 flute cutters and break very few. I am of course aware that I will probably be told that I'm doing it all wrong!!! G.

Not by me Geoffrey your cutting spot on IMO.

**deebo** · 21-05-2015

But what size cutter are you using?

**GEOFFREY** · 21-05-2015

Originally Posted by deebo

But what size cutter are you using?

6mm cutters and forgot to add that I cut in a single pass.

**Fivetide** · 20-02-2013

Thanks Jazz comprehensive as always mate :) I don’t think I have the skill to make a plate, but when I have the money I might ask someone to build one for me. I’m as usual over complicating things, maybe I’ll just get some 6 mm ball nose single flutes and do both clearance and finish with it ?