Setting Depth of Cut for V Bits and Ballnose bits

[Fleming]

If you are going to do a profile cut using a Vbit or ballnose bit and the depth is such that you want to do it in passes then you normally would go to the Specify Pass Depths window and enter the number of passes and/or set depths for each pass. This works well for endmills but because of the geometry of V and ballnose bits this is not the best strategy.

Example: let's say you have a 90 deg V bit and you want to profile cut .5" deep but you want to do it in several passes (let's say 5 passes) to minimize the stress on your machine and get a cleaner cut. Your first instinct is to simply go to the Specify Pass Depths window and set it for 5 passes which automatically sets .1" of depth for each pass. BAD STRATEGY! WHY? Because of the geometry of the bit you will be clearing only 2% of the material on the first pass/cut, 6% for the 2nd cut, 10% for the 3rd pass, 14% for the 4th pass, AND 18% for the final pass!

Just the opposite of what you really want to do which is take out the most material on the first few passes and clean up with the final pass.

According to the geometry calculations the strategy of removing 20% of the material during each pass would require the following 5 depth settings for a 90 degree V bit cutting .5" deep in 5 passes:
1st .22 deep
2nd .32 deep
3rd .39 deep
4th .45 deep
5th .50 deep

Of course these setting will change depending on the bit geometry, number of passes, and total depth to be cut and the math calculations are not easy but as long as you understand what is happening and the general pattern shown above
you can get better results. For instance the rule of thumb I use for 3 passes is 50% of depth 1st pass, 80% depth for 2nd pass, 100% for 3rd pass.

Maybe Vectric in the future will put an option on that screen which sets the depths for each pass based on the geometry of the bit! Till then use the above rule of thumb.

Happy cutting!

[FixitMike]

The VCarve toolpath makes multiple passes based on the pass depth setting to cut as deep and wide as necessary. Read the Help-Help Contents for the toolpath to see what it does.

"Multiple z level passes will be automatically calculated where the tool needs to cut deeper than its Pass Depth specified in the Tool Database."

[Fleming]

FixitMike,
You are correct but that is not the issue I was addressing. A Vbit by the nature of its shape cuts differing amounts of material depending on depth and the amount of material cut is related geometrically to the shape of the bit.

An endmill cutting .1" at first pass (out of 5) removes 20% of the total material (.5) to be cut and 20% for each additional pass. A Vbit with the same settings only removes 2% of the material on the first pass and has to remove 18% of the material on the last pass. If you specify 5 passes for the Vbit the software specifies .1" of depth for each pass just as it does for the endmill but the material removal for each pass is vastly different for the two bits. The window for setting passes does allow you to set a different depth for each pass but if you want that Vbit to have equal material removal per pass you need to use the rule of thumb I suggested.

Reread my analysis and let me know where I am confusing the issue so I can correct.

Thanks,
Paul

[GEdward]

I understand your argument but I don't quite understand your math. If your material removal analysis is correct, then 2% + 6% + 10% + 14% + 18% = 100%?? My math can be fuzzy at times, especially when I do it in my head, but 2+5+10+14+18=50. You've only removed half the material and managed to arrive at full cutting depth? What you are asking for, as I understand it, would be an option to manage pass depth of a cutter based on load management. I'm sure it could be done, especially for basic geometric shapes, but things could get interesting trying to refine the math to accommodate chip lead management for something like radius v-bits if the radius is not tangent to Z and/or the horizontal plane.

Ed

[FixitMike]

Sort of. After the V bit makes the first passes, the next passes don't have to remove the material that the first pass removed. They only cut into the material that is left at the specified pass depth. However, the pass depth is calculated from the bottom of the valleys of the previous passes, and the bit actually cuts its pass depth plus the peaks left by the previous passes.

The heights of the peaks depend upon the V bit clearance pass stepover specified. So, changing this number will change how much material is removed in each pass.

[GEdward]

For a v-carve strategy it is true that the v bit clears all but the clearance pass step over remains at the bottom of each Z level pass. Thus the v bit has very little, if any, full profile contact at full depth. The original post was considering the profile tool path I believe. In that case, the last pass has the v bit cutting the full profile of both sides of the cut. The cutter has a substantially higher load on it than it did in the previous passes.
It would probably be more accurate to say that what he wants to do is to be able to have the software calculate the pass depth based on removing an equal amount of material with each pass. Five passes, each pass removing 20% of the volume of the finished cut with each pass.

Ed

[Fleming]

Ed,

You are correct, I posted the wrong column of numbers from my spreadsheet.
Very sorry for the confusion. The concept I was trying (poorly) to communicate is still valid.

The correct numbers for a 90 deg Vbit cutting .5" deep over 5 EQUAL PASS DEPTHS of .1 are as follows:

Pass #1 cuts 4% of the material, pass #2 cuts an ADDITIONAL 12 % (total of 16%) of the material, pass #3 cuts an ADDITIONAL 20% (total of 36%), pass #4 cuts 28% (total of 64%) and pass #5 cuts 36% of the material (total of 100%).

According to my calculations (math is hard when you are old!) to get roughly EQUAL MATERIAL REMOVAL of 20% per pass for the scenario above, the first pass should be at depth .22", the second at .32", the third at .39", the forth at .45" and the final at .5"

Hope this makes things clearer instead of more murky.

[FixitMike]

Well, I certainly mis-read the original post. Profile, not Pocket or VCarve toolpath!

[TReischl]

...... Till then use the above rule of thumb.

Happy cutting!

Nah, it has not been an issue for me in the last 14 years.

[adze_cnc]

If your material removal analysis is correct, then 2% + 6% + 10% + 14% + 18% = 100%??

Yeah, I'm not so sure about the original maths. I suspect what the original poster was doing was taking a particular depth as a percentage of the total depth then adding the previous level.

• .1 / .5 + .0 = 0.2
• .2 / .5 + .2 = 0.6
• .3 / .5 + .2 / .5 = 1.0
• .4 / .5 + .3 / .5 = 1.4
• .5 / .5 + .4 / .5 = 1.8

Each result is then divided by 10 to get the decimal which is converted to the percent (e.g. 1.8 / 10 = .18 which is expressed as 18%).

But I don't thinks it's quite so simple. Let's reduce this problem down to using a 90 degree v-bit to drill down 1/2 unit deep (i.e. no lateral movement). This will give you a cone-shaped hole 1/2 unit high (h) with a radius (r) of 1/2 unit.

We'll use the same 0.1 unit depth increments. The volume of a right regular cone is: \pi * r * r * (h / 3)

At 0.5 units we're removing 0.1309 cubic units (u^3) in total.

If we were to independently drill 5 cones we'd be removing these volumes:

• 0.1 depth is 0.0010472 u^3
• 0.2 depth is 0.0083758 u^3
• 0.3 depth is 0.0282740 u^3
• 0.4 depth is 0.0670210 u^3
• 0.5 depth is 0.1309000 u^3

But we're not doing that. Each depth will be removing the amount of material less the amount that has been removed previously. Once we have that number we can divide by the total to be removed to get a percentage of what has been removed in that pass compared to the total amount to be removed.

For example: on the last pass the cone at 0.4 deep is not there. So the material we need to remove is 0.1309 u^3 - 0.0670210 u^3 = 0.063879 u^3.

The percentages of the material removed compared to the total material are:

• 0.1 depth is 0.8%
• 0.2 depth is 5.5986%
• 0.3 depth is 15.2010%
• 0.4 depth is 29.6005%
• 0.5 depth is 48.7998%

All that adds up to: 100.0044% (close enough).

What if we use a 90 degree bit to cut along a 10 unit long line?

The total material removed will be the cone we already have (half on one end of the line and half on the other) plus a trough (a right triangular section extruded 10 inches). Or 0.1309 + (0.7071 * 0.7071 /2 * 10) = 2.6299 u^3.

The 0.7071 is the length of the side of the cone from base to tip from the image below.

The material to be removed on the last pass will be this less the cone plus trough at 0.4 units deep. This is 1.667021 u^3.

The percentage (2.6308 - 1.667021) / 2.6299 * 100 = 36.6344%

Of course, my numbers are strictly based on total amounts removed for each pass. Really you'd have to do some weird calculations based on chip-load and the varying speed along the length of cutter at depth (e.g. for a cut at .5 units deep the bit edge at the surface of the material is moving faster than down at 0.5 units).

There may be errors above but my brain has turned to mud so it is what it is.

[Fleming]

adze_cnc,

Thanks for your more through analysis of total volume of the cone - that math is above me.

The only point I was trying to make is that using a set series of pass depths for Vbits and ballnose is not the same as using that setup for a straight edged endmill in terms of material removal per pass. For small less rigid machines one can get a cleaner and more accurate cuts if one takes into consideration what is happening in terms of material removal (& stress on the bit and machine) for each pass.

Much appreciation to all who contributed to this discussion. I have learned a lot.

Paul

[jay pieper]

Very interesting discussion...
Kind of reminds me of the old tv show Hee Haw
They told Junior Samples about Pi R square in math:
Juniors reply was Pie are Round.
So there you go!!!