[nadsab]

Hi,

Does anyone know what the maximum diameter end mill can be run on a Tormach PCNC 1100?

Thanks.

[MFchief]

If you mean a standard straight shank end mill, not a face mill or a fly cutter, then I would say 3/4". You can buy R8 collets in 7/8" and 1", but they are generally consider for light duty because there isn't much meat in the collet with a hole that large. I think an end mill in those sizes wouldn't be "light duty" if you where taking a cut large enough to need that size tool. YMMV

Terry

[Zetopan]

Does anyone know what the maximum diameter end mill can be run on a Tormach PCNC 1100?

Your question lacks important details. I have a lot of 1.25" end milling cutters and they work fine. I also have 1.5" and 3" carbide insert cutters. Many of my end mill sizes above 1.0" require tool holders, but many of them also have reduced diameter shanks.

[SCzEngrgGroup]

If you mean a standard straight shank end mill, not a face mill or a fly cutter, then I would say 3/4". You can buy R8 collets in 7/8" and 1", but they are generally consider for light duty because there isn't much meat in the collet with a hole that large. I think an end mill in those sizes wouldn't be "light duty" if you where taking a cut large enough to need that size tool. YMMV

Terry

R8 collets do not come over 3/4". The spinde bore is only 1", and a 3/4" collet only have about 1/16" of "meat" on the straight section, due to the relief on the outside of the collet. R8 endmill holders are available up to 1.25", and there may even be a few larger than that, but they're certainly not common. From a practical/useful standpoint, over 1/2" is probably the point of diminishing returns with a 1.25HP spindle. Larger tools can be used, but would have little or no advantage, except perhaps for very deep pockets, where the larger diameter will help with tool rigidity.

Regards,
Ray L.

[nadsab]

If you mean a standard straight shank end mill, not a face mill or a fly cutter, then I would say 3/4". You can buy R8 collets in 7/8" and 1", but they are generally consider for light duty because there isn't much meat in the collet with a hole that large. I think an end mill in those sizes wouldn't be "light duty" if you where taking a cut large enough to need that size tool. YMMV

Terry

Sorry I should have specified - I plan on using a ball nosed end mill, to machine aluminum plate.

[nadsab]

R8 collets do not come over 3/4". The spinde bore is only 1", and a 3/4" collet only have about 1/16" of "meat" on the straight section, due to the relief on the outside of the collet. R8 endmill holders are available up to 1.25", and there may even be a few larger than that, but they're certainly not common. From a practical/useful standpoint, over 1/2" is probably the point of diminishing returns with a 1.25HP spindle. Larger tools can be used, but would have little or no advantage, except perhaps for very deep pockets, where the larger diameter will help with tool rigidity.

Regards,
Ray L.

Thanks for the info! So - I read in the manual that the machine is 1.5 horse, so I am a bit confused why the R8 is only rated at 1.25HP?...

So it appears then that I should not go over 3/4 inch shank diameter to machine aluminum in this machine for practical reasons - is that the consensus? If so, are removable carbide type insert ball nose endmills available in a 3/4" shank size? To machine aluminum? I was hoping for a 4 flute design...but do they exist - is that practical or even advisable?

I ask this thinking it would extend tool life and allow the machine to max out the feed rate - which the manual claims is up to 110 ipm, and 90 ipm for Z. Given that, what kind of feed rate could I expect with this type of cutter?

For my application - very simple part - about a 5 x 7 piece of aluminum plate - all I am doing is machining a concave shallow spherical dish on one side of aluminum plate, and on the other side a convex spherical surface - spherical radius about 30" for both.

[nadsab]

Your question lacks important details. I have a lot of 1.25" end milling cutters and they work fine. I also have 1.5" and 3" carbide insert cutters. Many of my end mill sizes above 1.0" require tool holders, but many of them also have reduced diameter shanks.

Sorry about lack of details I added more in the other two posts.

Oh so - you are saying I could get an oversized cutter that only has a 1/2" or 3/4" shank diameter for the collet. So you are saying I could possibly get up to a 3" diameter carbide insert ball nosed type end mill that has a 1/2 inch or 3/4 inch shank? That would be great. I am assuming that this would vastly reduce the number of passes, and thus the machining time. I would love to get that down. Plus extended tool life.

I ran some simulations on Cut3d, and I was getting anywhere between 1.5 hour and up to 24 hours or more for this part depending on how I set the feed rates for roughing and finish passes. The largest cutter I ran on the simulation I think was 5/8".

So I am assuming if I went with over a one inch cutter, I could get the machining time down to below an hour since I could increase the stepover due to the larger size cutter? Is that correct or practicle?

[R.DesJardin]

Yes, it's 1.5hp. From what I understand you described for your part. I would use the Tormach 17mm or 25mm insert cutter to rough out the feature, these thing remove massive amounts of material fast. Then finish with a ball nose cutter or ball nose insert cutter that Tormach sells. The larger radius is nice for cutting curves but stepover is the key, The less stepover with the largest radius the better finish, the better finish the more time it takes.

[nadsab]

Yes, it's 1.5hp. From what I understand you described for your part. I would use the Tormach 17mm or 25mm insert cutter to rough out the feature, these thing remove massive amounts of material fast. Then finish with a ball nose cutter or ball nose insert cutter that Tormach sells. The larger radius is nice for cutting curves but stepover is the key, The less stepover with the largest radius the better finish, the better finish the more time it takes.

Thanks. Pardon my ignorance I am a newbie as far as machining is concerned, by the 17 or 25 mm insert do you mean an endmill with removable carbide inserts? Or a ball nose with removable inserts?

What's the largest ball nose cutter with removable inserts I could use on this machine? Also - if I increase the number of flutes does that reduce my machining time? Is approaching 100 IPM possible with a cutter at or near 1 inch diameter (not shank but the cutter diameter itself)?

If I use say for example a 1 inch ball nose cutter on the finish cut, with around a 2% stepover, what kind of tolerances can I expect on a 30 inch spherical dish radius - in regard to surface finish? Are we talking around +- .002 or way more than that?

[Zetopan]

I could get an oversized cutter that only has a 1/2" or 3/4" shank diameter for the collet.

0.75" shank sizes are readily available for cutters with up to at least 1.25" diameters.

So you are saying I could possibly get up to a 3" diameter carbide insert ball nosed type end mill that has a 1/2 inch or 3/4 inch shank?

No, I did not say that. My 3" diameter 45 degree carbide insert cutter has an integral R8 taper. I have no idea what maximal diameters are available for ball nosed carbide cutters that would fit an R8 taper.

I am assuming if I went with over a one inch cutter, I could get the machining time down to below an hour since I could increase the stepover due to the larger size cutter

That would depend on the depth of the cut and the resulting spindle HP loading.

[Zetopan]

R8 collets do not come over 3/4".

Actually, 25/32", 13/16", 27/32", and 7/8" bore R8 collets are also available. Their bores are shallower for obvious reasons. I would be quite reluctant to mount a large cutting tool in one, but they do work just fine for vertical lathe work.
Enco - Guaranteed Lowest Prices on Machinery, Tools and Shop Supplies

R8 endmill holders are available up to 1.25", and there may even be a few larger than that, but they're certainly not common.

They go up to at least 1.5" bores.
Enco - Guaranteed Lowest Prices on Machinery, Tools and Shop Supplies

From a practical/useful standpoint, over 1/2" is probably the point of diminishing returns with a 1.25HP spindle.

The Tormach PCNC1100 has a 1.5 HP continuous spindle rating and it can provide up to 2 HP for a limited time. The main reasons why I have large diameter cutters on my PCNC1100 are for the rigidity with long lengths, and due to the limited eBay buyers market for the larger sizes you can get brand new ones ridiculously cheap. All of my brand new Israeli made 1.25" end mills only cost me $4 each. They also happen to have a left handed helix, but the Tormach spindle doesn't care since it is reversible.

[MFchief]

Here's a Tormach 3/4" and a std 7/8", you can see the reduced amount of metal in the larger one. I think you can also see the step inside to keep from reducing the wall of the collet even further.
Sorry not the best lighting. LoL.
Terry

[TurboStep]

For my application - very simple part - about a 5 x 7 piece of aluminum plate - all I am doing is machining a concave shallow spherical dish on one side of aluminum plate, and on the other side a convex spherical surface - spherical radius about 30" for both.

I'm presuming you expect to lay the plate flat on the mill. In which case the above figures would indicate that the centre of the finished surfaces would only be about 0.3" above, or below the corners of the plate. Is this correct?
If so, roughing out this amount of material should take no time at all. You won't need a large end mill for this operation, I'd use just a normal (non ball end) end mill for this, and HP won't be an issue either. The problem starts with the finishing. The concave or convex surface is very shallow, so if you intend to hold the plate horizontally you'll only be using the very tip of the ball mill, especially in the centre of the plate where the surface would approach horizontal. This is not good practice for a ball end mill as only the very tip of the ball mill will be used, most of the end mill won't be used at all. The working diameter of the end mill will therefore be much smaller than actual diameter. This will seriously affect your surface feed (sfm) which will reduce to zero at the very centre. I would consider tilting the plate to 30-45 degrees to avoid using the tip of the ball mill and use the features of the CAM to follow the surface contours. You'll be able to maintain higher feed rates and you could use either a toroidal end mill or a ball end mill, either of which are available with inserts from Tormach (see the last 2 types here: http://www.tormach.com/product_tts_insert.html).
Step

[nadsab]

Thanks for all this great info folks. I recently was told that for aluminum, Tormach does not recommend using anything larger than a 3/4 inch shank, and a one inch ball nose cutter head - mainly because of the HP limitations for this machine.

So from what I am hearing, I should not use more than two flutes on a cutter for Aluminum mainly because of the chips and aluminum tends to gum up - is this correct?

[Steve Seebold]

R8 collets do not come over 3/4". The spinde bore is only 1", and a 3/4" collet only have about 1/16" of "meat" on the straight section, due to the relief on the outside of the collet. R8 endmill holders are available up to 1.25", and there may even be a few larger than that, but they're certainly not common. From a practical/useful standpoint, over 1/2" is probably the point of diminishing returns with a 1.25HP spindle. Larger tools can be used, but would have little or no advantage, except perhaps for very deep pockets, where the larger diameter will help with tool rigidity.

Regards,
Ray L.

I beg to disagree with you Ray, I have owned R8 collets that are 7/8 diameter and McMaster shows one 1 inch diameter.

[SCzEngrgGroup]

I beg to disagree with you Ray, I have owned R8 collets that are 7/8 diameter and McMaster shows one 1 inch diameter.

Clearly so, but, as pointed out, they are very "shallow", so probably not well suited to heavy work.

Regards,
Ray L.

[AUSTINMACHINING]

Thanks for all this great info folks. I recently was told that for aluminum, Tormach does not recommend using anything larger than a 3/4 inch shank, and a one inch ball nose cutter head - mainly because of the HP limitations for this machine.

So from what I am hearing, I should not use more than two flutes on a cutter for Aluminum mainly because of the chips and aluminum tends to gum up - is this correct?

Depends on DOC etc. I use a 4 flute .25" ball mill @ 6000 RPM and 40 IPM for finishing 3D surfaces. I rough using a standard end mill leaving .01" of stock. The proper way would be two passes (Semi finish and leave ~.003" for final finish), but for my needs, a single pass works fine.
https://www.youtube.com/watch?v=hMzm8tnnVh0

[dic_tools]

Hi

There are different sizes and shapes of end mills. I also used a roughing and finishing end mill with an overall length of 90-210mm

DIC TOOLS INDIA


https://dictoolsindia.com/hss-cuttin...-end-mills.php