30 Taper Machines: How do you estimate end mill downforce?

Hello,

I'm looking to replace soon my MiniMill with a Brother Speedio. I was told that is very important watch for the downforce generated by large / long end mills, using HSM tool paths, so it's better to make steps, instead using the full cutting length.

As an example, I'm sharing 2 screen-shots from the same part with two different scenarios. Notice that everything is in metric, at exception the end mill diameter (5/8").

Picture 1: Using the all the cutter length, higher feed, and lower engagement.
Picture 2: Using 3 steps, lower feed, and higher engagement.

Is there an easy way to estimate the downforce generated in each case? What option do you think it will be safer? Do you think is possible to have the enough downforce, to pull the tool holder out of the spindle?

Just trying to change the 'chip' from 40 taper, and be able to use the Brother the safest way possible. The good thing is that I don't run very often this type of parts, so I'm not concerned about cycle time. Safety first.

Thanks,

Ricardo

Not sure about the " down force" part of your question. But I will tell you one thing. If you want to stay safe and cautious follow the " 1/2 shank and under rule". Try your best to follow this and you will be less likely to break a retention knob or pull out a tool. 5/8 and larger are at a whole other level as far as rigidity and power needed. I am not saying you can't run tools larger than 1/2, just than when you do be aware that you should be cautious.

Customer wanted to use a 5/8" end mill to do some simple pocketing. I recommended to use a 1/2 cutter. He said 5/8 will be a lot quicker, " it only needs to mill .03 deep" he said. I asked how do you know it will only mill .03 deep. What if part is not clamped properly? What if part was sitting on a chip while clamped?

If you have something to estimate the cutting force (HSMadvisor or whatever) and know the helix angle of your endmill, you can trig out the downforce.

Honestly with long endmills vibration gets you well before anything pulls out on a 30 taper. Carbide corncob roughers are your friend.

If you had under 400-500 lbs of drawbar force you may want to think about this, with 800 lbs and up it won't be an issue. If your holding parts in a vise generally the part will move long before anything else, other than endmill in collets. You really are worrying about problems that don't exist. The biggest drawback with 30 taper holders is you are limited on how hard you can push long gage length holders.

I don't agree with Frank on the idea that 5/8" is too big for a 30 taper, at least not in my 30 taper mill. Gage length is CRITICAL!!!!!

For heavy stock removal in aluminum I use a 3/4" corncob mill. The only hesitation I have with it is pulling a part out of the vise, nothing to do with it being held in a 30 taper holder. Sure wish they could be made stubby but the tapers are just too small.

DavidScott said:

For heavy stock removal in aluminum I use a 3/4" corncob mill.

Click to expand...

I don't think the advice to not run 5/8" tools is that the machine can't do it... but has more to do with the risk/reward ratio.

60% of my time in the Robodrill is prototyping. I've run a dozen different parts in a day. I stick with 3/8" tools because I know if I fat finger a feed rate, or stepover value, or fuck-up the stock measurement, the worst that's gonna happen is a broken 3/8" rougher. Make the same mistake with a 5/8" tool, and I'm now looking at possibly trashing a spindle.

Now, if I was dialing in a production job and 5/8" tool to do something I needed, and was very cautious, and had full production Bozo Prevention Measures implemented? I would totally do it.

Only way you're going to get downforce from and endmill is by using a LH helix tool with a RH flute.
May actually be a competitive advantage for such a tiny toolholder; force the holder up into the spindle rather than gambling when a regular endmill will pop that Ø.25" retention knob.
Not sure how accurate one can "calculate" down force. One would have to take edge contact forces and account for helix angle of the specific endmill you're using today. Seems overly academic/impractical to me.

You gave no information except 30 taper and 5/8" endmill. How tall is the part? What material is the part? How are you holding the tool? You running a 60º helix 10 flute for Titanium? Or a 35º helix 3 flute for aluminum?

I will look at the corncobs. Right now I'm roughing and finishing with the same tool, because I don't have more pockets in the tool changer.

The 5/8" will be replaced for a 16mm, and hold in 45 mm gage length tool holder, which it's the shortest I found.

I'm not using 5/8" to save time. The surface finish is better, and I think I have a few more rigidity that the 1/2" for long tools (x4d).

gkoenig said:

I don't think the advice to not run 5/8" tools is that the machine can't do it... but has more to do with the risk/reward ratio.

60% of my time in the Robodrill is prototyping. I've run a dozen different parts in a day. I stick with 3/8" tools because I know if I fat finger a feed rate, or stepover value, or fuck-up the stock measurement, the worst that's gonna happen is a broken 3/8" rougher. Make the same mistake with a 5/8" tool, and I'm now looking at possibly trashing a spindle.

Now, if I was dialing in a production job and 5/8" tool to do something I needed, and was very cautious, and had full production Bozo Prevention Measures implemented? I would totally do it.

Click to expand...

Do you risk using a face mill when prototyping? My 2-1/2" facemill makes my butt pucker more than a 3/4" end mill.

Davidscott,
I never said that 5/8 is too big for a 30 taper machine. I am just trying to say that you should be aware of risks when running 5/8 tooling. Lets face the facts of a production enviroment. If this hasn't happened to you I will buy you lunch for a year.

wrong size material will be put in the machine
material will be put in wrong
part will slip from the vise
tool will break without you knowing and next tool will crash into it
program or tool offest error will bury the tool in a vise or the part

If you use 5/8 tooling take certain precautions. Add a probe to check material before running. Use short gage length tool holders. Have a tool load monitor system, etc.

Matt@RFR said:

You gave no information except 30 taper and 5/8" endmill. How tall is the part? What material is the part? How are you holding the tool? You running a 60º flute 10 flute for Titanium? Or a 35º helix 3 flute for aluminum?

Click to expand...

Sorry, I just found out the pictures I posted are too small!

The part is 68 mm tall (2.68").
Aluminum.
Hydraulic tool holder.
45º 3 flutes.

I use an occasional 5/8" or 3/4" tool on my Speedio, but only for finishing, or in plastics. In Al, I use a lot of 1/2" and 3/8" for roughing and with those tools I go full spindle load when feasible, and have never seen evidence of retention issues.

The one time I saw a retention problem was with a steel part, using a 1/2" endmill and HSM toolpath.

Regards.

Mike

riabma77 said:

Sorry, I just found out the pictures I posted are too small!

The part is 68 mm tall (2.68").
Aluminum.
Hydraulic tool holder.
45º 3 flutes.

Click to expand...

2.68" tall? Yea, I can see why you would want to go 5/8" with that.

I take it you want super clean walls without a multi-stepdown set of marks?

The most efficient way to do this would be with 3 tools. First would be an adaptive clearing, running balls out, with a 1/2" aluminum rougher with a 1.25" LOC to get you halfway down the part very quickly, in one of Frank's super short gauge length side lock holders. Second tool would also be in Frank's side lock, but an extended reach reduced neck rougher to clear out the lower half of the material using adaptive strategies.

Finally, bring in that big 5/8" bad boy in the hydraulic for a perfect wall finish.

In production, hitting the top with the low-risk 1/2" tool is going to make sure any bozo mistakes with stock size or workholding won't be fatal.

gkoenig said:

The most efficient way to do this would be with 3 tools. First would be an adaptive clearing, running balls out, with a 1/2" aluminum rougher with a 1.25" LOC to get you halfway down the part very quickly, in one of Frank's super short gauge length side lock holders. Second tool would also be in Frank's side lock, but an extended reach reduced neck rougher to clear out the lower half of the material using adaptive strategies.

Finally, bring in that big 5/8" bad boy in the hydraulic for a perfect wall finish.

Click to expand...

I do this same sort of thing ... but am sad that Schunk doesn't seem to offer a 5/8" Tendo hydraulic in BT30.

Having said that, I think unfortunately anything with 2-3/4" flute length is "An Endmill Too Far" for a 30-taper regardless of how you hold it. I'm happy to be proven wrong as I like to extend the capabilities of my Speedio, but this one seems like a stretch when I look at the mass the Speedio has in the general spindle area compared to a 40-taper machine.

Regards.

Mike

Finegrain said:

Having said that, I think unfortunately anything with 2-3/4" flute length is "An Endmill Too Far" for a 30-taper regardless of how you hold it. I'm happy to be proven wrong as I like to extend the capabilities of my Speedio, but this one seems like a stretch when I look at the mass the Speedio has in the general spindle area compared to a 40-taper machine.

Click to expand...

This sort of application is what the Big+ option is for. It'll rough that fine, but the 5/8" finisher will have to run probably a bit slower than one would like to get the walls perfect. It's one of those BT30 applications where you'll wind up with one operation being kinda inefficient, but you'll make up for it across the rest of the part.

Here is the data I was thinking for roughing and finishing with the same tool (5/8"):

1 step @ 68.1mm (2.68")
3690 rpm
2435 mmpm (96 ipm)
Step over max: 0.37mm (0.014")


But If I go "nuts" roughing with a 1/2":

3 steps @ 22.7mm (0.89")
10728 rpm
4470 mmpm (176 ipm)
Step over max: 2.47mm (0.097")

Do you think the light cuts with the 5/8" creates more downforce than the 1/2"?

If the best approach is to use different tools for roughing and finishing, what do you think about the integral indexable end mills? Any pros or cons versus corncob roughers?

I have one production part that uses a reduced shank 1/2" end mill with a 3.5" stick-out on a speedio, cutting 6063 aluminum, so it can be done, but it sounds like unholy hell when it runs.

You will want a big plus spindle for that tool if at all possible.


Your first scenario is 3.6 cubic inches per minute
Your second scenario is 15 cubic inches per minute.

That's... not a small difference. Why would you want to rough 4x slower using a bigger, more expensive tool?

Comatose said:

I have one production part that uses a reduced shank 1/2" end mill with a 3.5" stick-out on a speedio, cutting 6063 aluminum, so it can be done, but it sounds like unholy hell when it runs.

You will want a big plus spindle for that tool if at all possible.

Click to expand...

I know. I used a lot the 1/2" MariTool's reduced shanks, but the finish wasn't great (step marks, etc...). If I use it again for roughing, probably I will have to cut the shank to fit in a 60mm SK or similar.

riabma77 said:

Here is the data I was thinking for roughing and finishing with the same tool (5/8"):

1 step @ 68.1mm (2.68")
3690 rpm
2435 mmpm (96 ipm)
Step over max: 0.37mm (0.014")


But If I go "nuts" roughing with a 1/2":

3 steps @ 22.7mm (0.89")
10728 rpm
4470 mmpm (176 ipm)
Step over max: 2.47mm (0.097")

Do you think the light cuts with the 5/8" creates more downforce than the 1/2"?

If the best approach is to use different tools for roughing and finishing, what do you think about the integral indexable end mills? Any pros or cons versus corncob roughers?

Click to expand...

Length of cut has a bigger effect than width vis-a-vis pullout torque.

This is aluminum? I would be using all 16k on the spindle at all times, there is effectively no speed limit for aluminum with carbide (unless we're talking about some funky finishing stuff in some limited circumstances).

The extended reach aluminum roughers tend to have .75" flute lengths on a 3.375" LBS shank. Plugging those numbers into HSM and fiddling with the variables around my experience, I get a cut that looks like this:

Destiny Diamondback 1/2" 3.375 LBS Rougher:
- 16k RPM
- 375 IPM
- .75" Depth
-. 0.050" WOC

That would be a ~4hp cut, which is a good measure of just how much stress you're putting on the spindle, so totally within the realm of the BT30. It also has an decent 13.78 cubic inch MRR, which isn't horrid given the limitations.

For comparison though, let's see what the first 1.25" of material removal look like if we use a standard rougher and lean on the fact that the Speedio has a 1.4 second chip to chip time, making the tool change an irrelevant factor in our overall cycle time:

Diamondback 1/2" 1.25" LOC rougher:
- 16k RPM
- 200 IPM
- 1.25" Depth
- .109 WOC

... Doubles our MRR, and a dialed back feed rate gives damn near double the MRR of the long cutter (28 cubes a minute).

But for fun, let's take the whole thing in one depth and see what we get with a 1/2" roughing tool:

Diamondback 3/4" 3" LOC Rougher:
- 16k RPM
- 162 IPM
- 2.89 DOC
- .054 WOC

Gives us 25 cubes, running at a higher 7hp for the cut, which is starting to really push it on a BT30 when you're handing so far out of the bottom of the spindle. I would probably back off the feed till we're at a 4hp cut, which drops the cubes down to 16. Humph!

You buy a Speedio because it's fast, but you need to change your way of thinking a bit to get it to work. Tool changes are essentially *free* of impact on the cycle time, so use that to your advantage and run the optimal tool for the task at hand.

Diamondbacks are rougher/FINISHERS, leaning towards finsiher. A corncob rougher is way less stress on everything! I have used plenty of Diamondbacks but for roughing only they leave a lot to be desired. Try it full depth using a 1/2" corncob rougher, say a MA Ford, and don't be shy about stepover. Don't just go full rpm, less rpm with a bigger chip load may work better, with that cutter you can go up to .05" per tooth easily.