Cut per depth for 3/4 inch oak

[cgilreath]

I am using a whiteside 1/4 shank 1/4 cutting diameter spiral down router bit (RD2100) on BOBSCNC Evolution 4 with a dewalt dpw611 router. I am trying to cut all the way through 3/4 inch oak. My settings have been .0625 at a feed rate of 20ipm and around 22,000rpm. Sometimes the bit bites in the corners and digs into the wood and damages it. Does anyone have better luck with that same setup?

Thanks! Chris

[Rcnewcomb]

Try changing the Conventional/Climb setting. If the edge quality on the scrap is better than the edge quality on the part, then you want to switch your climb/conventional setting.

BTW, 22K RPM is too high when you are moving that slow. It builds up heat and reduces tool life. Your bit may already be dull as a result.

You will want to decrease your RPMs and/or (probably both) increase the feed rate.

[cgilreath]

Thanks. I have tried both Conventional and Climb and i get less chatter with conventional. The recommended maximum rpm per Whiteside is 24,000 so that is why i stay at 22,000 but may need to lower the rpm so it is not as violent when going into corners where the wood surrounds more of the bit thus creating kickback. For cutting all the way through 3/4 oak, do you think it is better to increase cut of depth from .0625 to .08 and leave at 20ipm and rpm to around 20,000 or leave at .0625 stay at 20ipm and put to 20,000 rpm? Again, I want to remove the violent kickback i get when it goes into an inner corners like shown circled below. T

Thanks.

[mrmfwilson]

Generally when I use a 1/4" 2 flute spiral bit, I cut at .125" depth at 14000 rpm/ 50-75ipm in most wood. If I cut a .0625 depth I would up the feed rate to 100 at least. On a profile I use the ramp option at a specified length. Usually between 1 and 2 inches so that the tool moves slowly down into the material. I don't have the same setup as you and I don't know about your machine construction. If you are only cutting .0625, you need to slow down the rpms to something around 14000 rpm @ 20ipm. You might be able to double the feed rate. Although your spindle speed is too high that should not make it jump around unless you have dulled the tool and it is grabbing the material, not cutting it. You will definitely dull a tool running it at a high rpm and slow feed rate. Most wood bits are made to run between 12000 and 16000 rpm. Unless you want to run at 200ipm or higher. Then you will need to turn up the rpms.

Have you successfully cut other wood without problems? Have you checked for backlash?

I guess another problem might be that if you used a DXF file to start from, each vector will be split into many small vectors. This can sometimes cause the machine to jump around or make very sharp movements because it is just cutting a small segment at a time.

[cgilreath]

Thanks for the feedback mrmfwilson. The only other wood I have done the same design was mdf for a proof of concept and no issues.

The vector created to cut all the way through was an offset I created from a bitmap that I used the option to trace bitmap. You are correct the small vector cuts I have highlighted move at a faster pace than the rest and those are the main ones that are violent and grab the bit sometimes (even when I am using a fresh new bit). They are saves as one gcode file so don't know how to slow those down from the rest.

[Rcnewcomb]

They are save[d] as one gcode file so don't know how to slow those down from the rest.

That is a function of your control software, not the G-code. It may be a constant velocity setting or some other parameter.

Are you running Mach3, Mach4, or something else?

[cgilreath]

BobsCNC Evolution 4 runs GRBL1.1 firmware on the Arduino Uno. Here are the firmware settings:
Key Value Description
$0 10 (step pulse, usec)
$1 25 (step idle delay, msec)
$2 0 (step port invert mask:00000000)
$3 0 (dir port invert mask:00000000)
$4 0 (step enable invert, bool)
$5 1 (limit pins invert, bool)
$6 0 (probe pin invert, bool)
$10 1 (status report mask:00000011)
$11 0.01 (junction deviation, mm)
$12 0.002 (arc tolerance, mm)
$13 0 (report inches, bool)
$20 1 (soft limits, bool)
$21 0 (hard limits, bool)
$22 1 (homing cycle, bool)
$23 3 (homing dir invert mask:00000011)
$24 250 (homing feed, mm/min)
$25 2000 (homing seek, mm/min)
$26 250 (homing debounce, msec)
$27 5 (homing pull-off, mm)
$30 1000 Maximum spindle speed, RPM
$31 0 Minimum spindle speed, RPM
$32 0 Laser-mode enable, boolean
$100 80 (x, step/mm)
$101 80 (y, step/mm)
$102 400 (z, step/mm)
$110 10000 (x max rate, mm/min)
$111 10000 (y max rate, mm/min)
$112 2000 (z max rate, mm/min)
$120 500 (X-axis acceleration, mm/sec^2)
$121 500 (Y-axis acceleration, mm/sec^2)
$122 500 (Z-axis acceleration, mm/sec^2)
$130 610 (X-axis maximum travel, millimeters)
$131 610 (Y-axis maximum travel, millimeters)
$132 85 (Z-axis maximum travel, millimeters)

[Rob302]

When I cut thick pieces I have found for my machine that .125 pass depth, 50IPM and 9000RPM works great.

[cgilreath]

Thanks Rob302.

[mrmfwilson]

My first thought was the same as Rcnewcombs. That it was a controller or software problem. From what I can tell, not knowing what the normal settings, from these key settings everything looks normal. The 2 keys that I think might have an effect on the motion are the junction deviation and the arc tolerance. Those are so small I doubt if they are a problem. Assuming you have verified that the steps are correct the only other thing that could possibly cause a problem is the axis acceleration.

I would suggest tracing the bitmap instead of using the trace bitmap tool. That would eliminate any possible drawing problems. Use fillets where the tool will not fit into the corners. You can look at the gcode to see if there are any speed changes. I don't know why there would be if it is all one toolpath using the same tool.

Can you post the .crv file?

BobsCNC Evolution 4 runs GRBL1.1 firmware on the Arduino Uno. Here are the firmware settings:
Key Value Description
$0 10 (step pulse, usec)
$1 25 (step idle delay, msec)
$2 0 (step port invert mask:00000000)
$3 0 (dir port invert mask:00000000)
$4 0 (step enable invert, bool)
$5 1 (limit pins invert, bool)
$6 0 (probe pin invert, bool)
$10 1 (status report mask:00000011)
$11 0.01 (junction deviation, mm)
$12 0.002 (arc tolerance, mm)
$13 0 (report inches, bool)
$20 1 (soft limits, bool)
$21 0 (hard limits, bool)
$22 1 (homing cycle, bool)
$23 3 (homing dir invert mask:00000011)
$24 250 (homing feed, mm/min)
$25 2000 (homing seek, mm/min)
$26 250 (homing debounce, msec)
$27 5 (homing pull-off, mm)
$30 1000 Maximum spindle speed, RPM
$31 0 Minimum spindle speed, RPM
$32 0 Laser-mode enable, boolean
$100 80 (x, step/mm)
$101 80 (y, step/mm)
$102 400 (z, step/mm)
$110 10000 (x max rate, mm/min)
$111 10000 (y max rate, mm/min)
$112 2000 (z max rate, mm/min)
$120 500 (X-axis acceleration, mm/sec^2)
$121 500 (Y-axis acceleration, mm/sec^2)
$122 500 (Z-axis acceleration, mm/sec^2)
$130 610 (X-axis maximum travel, millimeters)
$131 610 (Y-axis maximum travel, millimeters)
$132 85 (Z-axis maximum travel, millimeters)

[cgilreath]

I have attached the .crv file. It says I am using a RU2100 but I am using a RD2100. The down spiral is not in database.

[mrmfwilson]

I don't see anything that should be causing the problems that you are describing. I used the BobsCNC PP and the GRBL PP. They produce identical files. The feed speed is constant throughout the gcode. 40ipm feed and 20ipm plunge. The lines could use a little cleanup with the node editing tool. Most of the lines are straight. I would remove any unnecessary points leaving just the end points before doing the offsets. I think that every point is a interpreted as a start/stop for the gcode. But that's just me being picky... Perhaps you could try and add more tabs to stabilize the piece better while the outline is cut? Otherwise it looks like it is a control software, hardware controller, or machine issue.

[cgilreath]

Thanks. That was my first design in Vcarve so am still learning the software. I was able to finish one plaque just now with the following settings: Profile cut all the way through at .0625 pass depth and feed at 15ipm at around 19,500 rpm.

It was slow and when crossing the grain you could hear it chatter. All with a brand new bit. I might have to stay with those settings for oak.

[Charlie_l]

Good news.
Did you notice how hot the bit got? Seems like those speeds would really heat it up.

[cgilreath]

No heat at all. I like Whiteside's all carbide bits.