[twocik]

I have a few jobs that require more metal removal and figured a GMT 2.5" FM45 could be my answer. I also noticed right after I order the 2.5", they also make a 3" FM45 that also has the same size 1" bore... This might be next on my list if the 2.5" works out.

I've always wanted to try and TTS this tool and finally have the need for it. A member here has already had success converting this tool, but not much documentation to be found. I'm going to document the process of the TTS conversion for those that might share the same questions.

I picked up a Glacern 2.5" FM45 face mill and a Shars 1" bore 3/4" straight shank last week (recommended from another user here). The Tormach 90° face mill has been great, but 1.5" isn't enough for some of my newer runs. GMT recommends a great starting point of 1500 SFM @ 0.01" per tooth feed rate. However I think this is based on machine with a 10HP or more. I'm also going to post my S&F test results.



So far the shank definitely needs to be shortened. Next I'm going to glue the TTS conversion ring and see how that holds up. My FM45 & inserts should be here some time today.


Here's what I was able to finish yesterday








Note - I removed the holder locking keys before I chucked it.















(not bad, .0003" RO)

[philbur]

The larger the diameter of the cutter the longer is the lever-arm and therefore the greater is the risk of pull-out when you are going for high removal rates.

With the TTS there is a good argument for going with relatively small diameter endmills using high rpm with big DOC and feed. Removal rate is dictated by horsepower employed, not by cutter diameter.

In addition large diameter cutters require relatively low rpms, this can put you in the VFD constant torque region - meaning a reduction in available horsepower and therefore a reduction in maximum material removal rate.

Phil

[twocik]

Face mill is in, putting it together now. :wee:



Hi Phil,
From my research you're dead on and is why I went with the GMT 2.5" FM45. From the GMT site, "Can be used on smaller machines thanks to the low horsepower requirements."


I don't plan on taking deep hard .08" - .25" cuts, but something like 0.03" - .04" at 2.5" WOC would be prefect. A few new parts I'm making have a .120" x 4"W carrier that I need to take off every time. At 250 parts with a 1.5" FM that can take a little bit of time to remove....



The Tormach holder is measuring in at 1.382" L (from ring lip to shank end). I designed my holder to just clear the TTS 1.5" measuring cylinder. The DIY TTS ring measures .2" in thickness and my tool holder with the ring installed is 1.475" (W/O TTS ring 1.662"). We'll find out very soon if I cut this shank too short. If I did I'll just order another from shars ($35) and cut that right below the draw bar.

[Andre' B]

The larger the diameter of the cutter the longer is the lever-arm and therefore the greater is the risk of pull-out when you are going for high removal rates.

With the TTS there is a good argument for going with relatively small diameter endmills using high rpm with big DOC and feed. Removal rate is dictated by horsepower employed, not by cutter diameter.

In addition large diameter cutters require relatively low rpms, this can put you in the VFD constant torque region - meaning a reduction in available horsepower and therefore a reduction in maximum material removal rate.

Phil

It takes a lot of horsepower to make full use of a large cutter.
We just finished a job on a mill with a 30HP spindle with a 2 speed gearbox. We were running a 2.5 inch face mill with the spindle at 70% load, could have easily increased the depth of cut and run it up over 100% but the part clamping was less then ideal and we did not want to push it.
We were taking 432 cubit inches of steel off each part and making all kinds of chips.

[twocik]

Here she is !














After testing with a few different hand codes, I was able to find a very nice finish at the depth and speed I was after. I'd say I was seeing about 50% - 60% on my spindle load meter.

full 2.5" WOC
2300 rpm
50 IPM
0.020" - 0.025"DOC

dry cut


No problems at all, extremely nice mirror finish ! I'll post a few pics soon.

[Steve Seebold]

I'm in the process of making TTS rings for all my 3/4 inch tooling.

I made them from 7075 aluminum. The O.D. is 1.500, the counter bore is 1.300 diameter X .125 deep and I made the hole .748.

If you make the hole .748, then you can heat the ring and drop it on, but you need to make sure it's where you want it when it cools because when it does cool and shrinks with .002 press fit, you ain't movin' it again.

[twocik]

Great idea Steve !

[Don Clement]

Nice job on the 2.5" TTS facemill. Thanks for showing us the way.

Don

[philbur]

Here's a calculator for that type of face mill:

mill calculator.

Phil

[David Bord]

Very nice looking piece... Really nice work on that. Id love to see the surface finish it produces. What is the MRR if you push the tool a bit?

David

[TXFred]

I'll bet that you can run a lot faster than that. That face mill isn't much bigger than the Tormach face mill, which can do 90 IPM at 3600 RPM, 0.020" DOC in aluminum.

[ame=http://www.youtube.com/watch?v=1IXgLPq_nFQ]Face Milling with a Tormach PCNC - YouTube[/ame]

[beanbag]

Just be careful not to do a full width ramp with this facemill, or you will risk stalling the motor.

[twocik]

Thanks guys ! Running a few more (top side) parts today and hopefully I can get to facing them. I'll post some pics soon


Phil checking that out now, very cool ! I've been using Machinist Apprentice, simple but works great for on the fly stuff.


"What is the MRR if you push the tool a bit? "

full 2.5" WOC
2300 rpm
50 IPM
0.020" - 0.025"DOC

dry cut

Not sure yet, but I'm thinking anything over the S&F I posted at .03" might be cutting it. I'm going to play with the feed a little more, but anything around 2300 rpm - 3500 rpm seems to cut with very good torque (again I was dry cutting...) I think when I plugged the info. in it said something like 1.7hp needed at .03" same settings.

[Rendrog18]

twocik,

Just wondering how this face mill is working out for you? I'm interested in buying one and was hoping for some feedback from you. Notice any tool pull out? Why did you choose to run dry cuts? Any extra info would be great.

Thanks!

[twocik]

Sorry I haven't had a chance to take photos and doc things, right now I'm finishing a job and should have more info soon. As for how it's working out, well lets just say I have 2x 15 - 25 lbs bags of chips waiting to be recycled. This tool is a beast and was worth every penny ! No pullout at all and I've been running it pretty hard and fast. I've even had a few G00 by accident and took it no problems.

As for dry cuts, you might be confusing the GMT FM 2.5" with the Tormach 1.5" FM.... I run both face mills with coolant, especially the GMT 45 degree FM on AL. Both are great tools to own and use them a lot.

[Rendrog18]

After testing with a few different hand codes, I was able to find a very nice finish at the depth and speed I was after. I'd say I was seeing about 50% - 60% on my spindle load meter.

full 2.5" WOC
2300 rpm
50 IPM
0.020" - 0.025"DOC

dry cut


No problems at all, extremely nice mirror finish ! I'll post a few pics soon.

This is why i was asking about running dry. So typically, you cut wet, was this just a test running dry? I'm thinking about a 2" Shars facemill and tts'ing it like you did. Looks to be pretty similar to the GMT. Though i have no doubt GMT has quality products.

[tbaker2500]

I didn't see any video from him, I only saw the Tormach video posted later in the thread, which was running dry.

[dbrija]

A small note... I have the same mill and a similar arbor, and instead of using a TTS conversion, while you have the arbor in the lathe parting off some of the shank length, just turn a relief in the arbor itself to clear the R8 collet (equivalent to adding the TTS without the extra stick out).

[Steve Seebold]

I remember back in the early 80's I used a cutter similar to this on a manual Bridgeport type machine, and after about 2 hours use, I had to replace the spindle bearings.

Just remember, your Tormach is a light duty machine and you don't want to have to put in a new spindle because your cutter beat up the bearings. I would rather take a little longer and use a smaller cutter.

I have learned over the years that I can remove more material using a shallow depth of cut along with a high speed and a high feed rate. The articles you read about volume mill in the trade magazines support this theory. I have seen a friend of mine cut 17-4 stainless at 1.999 depth of cut with a 1/2 inch end mill at 7,500 RPM and a .030 radial depth of cut at 90 IPM. I once saw 718 inconel cut the same way.

[Rendrog18]

Steve,

Would you believe that a 2" Shars 45 degree face mill to be that more of an impact on the spindle over the Tormach 1.5" 90 degree face mill? The Shars mill is only 1/2" larger but according to several manufactures, the 45 degree cutter requires less horsepower than the 90 degree cutters. If it requires less horsepower, wouldn't this mean that it is generating less force while cutting than its 90 degree counter part?

It seems to me that even though the cutter is larger, it wouldn't be putting much more, if any, load on the spindle if it is requiring less horsepower to use.

Am I'm understanding/looking at it wrong?