# G-Wizard and #101 and #102

I"ve known Gearotic for some time and yesterday I saw a deal that bundles gearotic and gwizard: http://www.cnccookbook.com/GWGearoticSignup.html. Since I wanted gearotic, I thought that paying \$7 for G-Wizard was worth it.

It was a pleasant surprise to see the Nomad listed. And now to my question. In the Feeds/Speeds calculator, what should I use for Cut Depth and Cut Width for the #101 and #102? The meaning of those parameters was not clear to me from the youtube videos. If somebody could shed some light …

Thanks,

Ric.

I believe these are in the Carbide Create tool library

Thanks Will. I installed the program, I couldn’t find a tool library. All I see is a library of shapes. I thought some information could be hidden in the g code, but it is encrypted (or encapsulated, I don’t know).

Listed as 0.125"diameter use half that for d.o.c. as a start per http://www.shapeoko.com/wiki/index.php/Materials#Overview and see http://docs.carbide3d.com/article/47-measuring-runout

1 Like

The geometry for the 1/8 bits that come with the nomad are:

Flutes = 2
Tool Dia. = 0.125
Shank Dia. = 0.125
Overall Len. = 1.5
Flute Len. = 0.5
Stickout (assuming it’s fully seated in the collet) = 0.72
Taper Angle = 90

For the ball nose select Ballnose and for the flat end mill select Normal

Cut depths and widths are purely dependent on the type of cut you are doing. For example, if you are doing a plunge into a pocket, then slotting it, you have no choice but to set the cut width = diameter of the cutter.

If you are not limited by the type of cut, lets say you are using adaptive clearing, and you want to maintain an ideal cutter engagement, then you want to use the cut optimizers (these are the little things next to the depth and width boxes).

At the end of the day, what really matters is what the machine can handle, what the cutter can handle, and what kind of finish you want. Here’s a good approach at making that happen:

1. set the HP Limit to ~0.03. Small machines like the nomad are limited by weight/rigidity and not by spindle horsepower.
2. Make sure your cutter geometries are entered correctly, especially stickout, because this is how tool deflection is calculated.
3. Decide if you are slotting, or using less of the cutter. Set your width based on high material removal rate (more of the cutter), or finishing (less of the cutter).
4. Select your surface finish between 1%-100% Rough.
5. Click Optimize near the cut dept. Select a deflection allowance based on what kind of cut you are making.
6. Make sure the solution converges and gives a reasonable answer. It’s tricked me before!
7 Use those cut parameters.

You’ll instantly notice that the roughing cuts recommended by GWizard are wayyyy more aggressive than what Carbide3D recommends. If you did everything correctly, don’t worry, the machine will handle it (assuming you compensated the horsepower for machine rigidity). You don’t have to worry about breaking/clogging a cutter with these calcs. It’s the whole reason my approach is based around deflection.

Troubleshooting:

1. If the cutter stops mid cut: Turn down the horsepower limit. You’re reaching the rigidity limit of your machine.
2. If a tool breaks: GWizard tricked you and the deflection calculation didn’t converge. You didn’t read carefully in the little box! Stop rushing!
3. Surface finish is bad: Take a more conservative cut, 25% or less.
4. Cutter stalled on plunge: Did you remember to enter the correct plunge numbers in the CAM software?
5. Cutter stalled on ramp: Set your ramp feedrate closer to the plunge feedrate.

By the way, this was a quick type, so not everything is perfectly explained here. I also oversimplify some things. Best thing to do is read a machinists handbook from cover to cover if you really want to know how to choose your cut parameters.

4 Likes

This is very helpful. I’m starting to realize that I have a lot to learn before I use the machine for the first time. I feel that with your valuable help I’m getting there…

This is excellent Jon! Thank you very much!

Ok, I followed your procedure but I’m not sure that my results are right. Here is what I am doing on GWizard:

1. Machine Carbide3d Nomad, Material: Plywood, Tool: Carbide3d #101. I was very careful entering the geometry as you suggested, I double checked by using metric (which is what I know) and imperial to verify that the tool matches the geometry you posted. (Issue: When I was creating the tool, I couldn’t set the OAL)
2. I set the HP limit to 0.03 as you suggested.
3. I leave Mfg and MiniCalcs alone.
4. I go to the Width field and set it to 0.0625. I notice that I can only set a value on the width field if the Depth field has a non zero value. Do you see that behaviour too?
5. I set the surface finish to 23%
6. I click on the optimize icon near cut depth. I get a red popup telling me the calculation is not possible. I played around changing RPMs, cut widths and depths until I finally could use the optimization. I got a value of 0.72 (exactly the stickout) for the depth and the width went to zero. Very suspicious.

It likely means you’re attempting a cut that just isn’t possible. This is why I always say check the result, because it’s fooled me like that before.

A few things, you should make your cuts more or less than half your cutter. If you cut at the centerline you will get a worse finish/burrs.

I don’t have the #101 tool in my crib, but I tried the optimization with a similar maritool bit and got:
Cut Width: 0.0375
Cut Depth: 0.3427
RPM: 10,000
IPM: 14.783
Plunge: 6.8

So I grabbed a piece of plywood and tried it. Result? There was a little chatter from the table, so I backed off on the depth to 0.32 (yes 0.32") and IPM to 14.0. Cut like a champ with good surface finish.

1 Like

Thanks again Jon. I don’t know what I’m doing wrong, I’m using your value for cut width and the depth optimization optimization tool gives me an error. I made a little video to show what I’m doing: https://youtu.be/QO4iIh1pEAQ. Must be something painfully obvious but I can’t see it.

Video is set to private so I can’t see

Silly me. Wanted to make it unlisted. Now it should be viewable.

Anyway, I sent the video to the developer. He acknowledged that there is a bug, he’ll look at it.