How Much Horsepower Do You Use - How Hard Can you Push It

[Bob La Londe]

I've been using the 1100 (PDB & ATC) quite a bit lately for squaring up the ends of stock 6061-T6511 aluminum blanks

with a 1/2" 3 flute

before moving them over to the little high speed machines. The other day I noticed the TTS holder had pulled quite noticeably from the collet.

I went back and retorqued the springs on the drawbar to finger tight plus 2.5 turns. So at a setting like that how hard can you push it and KNOW you won't pull tools from the spindle using the stock PDB setup. I'm getting ready to run some longer jobs and I can't have the tool holder walking out of the machine.

Similar Threads:

• Why is my horsepower so low
• How hard can I push this?
• How hard is to hard to push a VF-2 SS
• How hard can I push a drill ?

[popspipes]

My solution to it is to use 140# air pressure (2 stage compressor)
Tighten the drawbar until it just will release.
Then run the cutter just below the chatter point, chatter seems to be where the pullout starts for me.

I also use 1/4" cutters and smaller mostly as 1/2" seems to be a bit large for the machine's ridgidity.

I also grease the spindle taper and the taper on the R8 occasionally.

[jwatte]

FWIW, with a manual drawbar, I still had lots of pull-out trouble on the 1100 I used to use, when using 1/2" tooling in 6061, running it at yellow loads.
That machine wasn't particularly well maintained, so maybe the important bits for TTS weren't up to snuff (clean shanks, no grease on holding surfaces, but do put grease on compressive surfaces.)
But I had enough problems that I ended up using 3/8" where possible, just to avoid not knowing whether it would work.

[Bob La Londe]

Thanks guys.

I have read elsewhere and seen one video that 3/8 seems to be the anecdotal limit the authors have found with their 1100s, and that 1/2 tools tended to pull out the holder. I spent a good part of the day yesterday creating CAM styles for Tormach for 1/2 inch endmills (and others) and setting up a job. Now I feel silly. I tried to keep loads low and take advantage of chip thinning strategies. Now I am second thinking myself and considering changing those portions of the job to 3/8 anyway. I may run it just the way it is and see what happens. I'll have to supervise it with a hand over the e-stop I think. I have extra material to recut the job if necessary, and there is a certain inherent confidence to gain from failures. The thing is with the 1/2 inch tool I can do some operations (per my calculator) as efficiently as a smaller tool in the little Speedmasters. Even at the less than 100% loads I used. If I can run them it will make the machine competitive with its smaller faster brethren in the shop for some jobs.

If not, well then I delete the 1/2 inch tool from the tool table and CAM styles so I'm not tempted and work up a set of CAM styles to use a 3/8.

Well all that and I don't think I have any 3/8 Alu-Power end mills. LOL. I do have several 1/2 inch which I use a lot on the Hurco KMB1, and lots of 1/4 inch which are the primary roughing tools on the Speedmasters.

[SCzEngrgGroup]

Bob,

The limiting factor is going to be the PDB, NOT TTS itself. The Tormach PDB simply does not provide optimal drawbar tension, and if you push too hard, you will get chatter and/or pull-out. With proper drawbar tension (approx. 1000# more than the Tormach PDB provides), you will NEVER see pull-out. Unfortunately, there is no reasonable way to accomplish that with the Tormach PDB without replacing the large pneumatic cylinder with an even larger one, or, better still, with an air-over-hydraulic actuator. Barring that, the best you can do is make sure the all the PDB springs are well-lubricated with anti-seize, run the highest air pressure you can manage, and carefully adjust the PDB springs so the PDB can JUST barely release the tool. If you're using an ATC, you may find it occasionally fails to release on toolchange.

Regards,
Ray L.

[Paul-JB]

Just buy an extra TTS collet and send it to these guys have them coat the 3/4” ID... either W or #1
Carbinite Metal Coatings
When doing pull out prone work, I use 2 small strips of
.002 shim stock at the holder/spindle nose interface as a tell-tale. Soon as the shims fly out i can hit the stop before anything bad happens. Lot easier than trying to eyeball light coming through the gap!

[jwatte]

{code]The limiting factor is going to be the PDB,[/code]

I had the pull-out with manual tool change (no PDB.)
Then again, as I said, the machine wasn't very well maintained (shared workshop.)

[Bob La Londe]

Well my test run showed that the 1/2 inch end mill just won't do. I could see a step down in a roughing cut with every pass. Even when I turned feed way down from calculated I could see a thousandth or so. At calculated it was walking down newaht looked like between 5 and 10 thousandths over a 17 inch cut I was able to save the part, but only because I planned to machine the back off anyway. I'll just have to machine a little less off the back. I may change the machine setup later. For now I just set it aside and deleted it from my tool table on both the machine and my CAM software so I won't be tempted to run it. Interestingly the 3/8 I plugged in and calculated (I had one fast helix Alu-Power 3/8 new in the box in the back of my square end mills drawer) pushing at nearly the same horsepower loads had no issues with pullout. Even when pushed hard enough to chatter.

[R.DesJardin]

1/2" end mills are the devil. I run YG1 3 flute 3/8" roughers when I need to hog shapes or pockets, or the Tormach 17mm insert cutter for just get material gone on larger parts.

[wildwhl]

Well my test run showed that the 1/2 inch end mill just won't do. I could see a step down in a roughing cut with every pass. Even when I turned feed way down from calculated I could see a thousandth or so. At calculated it was walking down newaht looked like between 5 and 10 thousandths over a 17 inch cut I was able to save the part, but only because I planned to machine the back off anyway. I'll just have to machine a little less off the back. I may change the machine setup later. For now I just set it aside and deleted it from my tool table on both the machine and my CAM software so I won't be tempted to run it. Interestingly the 3/8 I plugged in and calculated (I had one fast helix Alu-Power 3/8 new in the box in the back of my square end mills drawer) pushing at nearly the same horsepower loads had no issues with pullout. Even when pushed hard enough to chatter.

I've experienced essentially the same, and the 3/8" Alu-power cutter is my go to for most roughing ops, unless I need something longer. Then I grab the 1/2" by same mfg. Key to making the 1/2" work is within the details shared above, and also a formula running around 3800 rpm (peak torque range) and pushing the load meter to the edge of green/yellow. Running 12 washers on the PDB I can stall the spindle with either 1/2" or 3/8" cutters before I get pullout - UNLESS - I somehow induce chatter. Then, depending on how clean and happy the TTS is I may still get pull out (flood coolant gets things pretty messy up in the ATC at times).

Bill

[hersh]

Have you tried the Shear Hog?

Also, if you are doing the same operation over and over, just hogging out material, and don't need to change tools, you could disable the PDB, go back to the shorter draw bar without the spring washers and run a normal R8 end mill holder. Its a pain, but better than worrying about pull out if you can justify the amount of run time you can get before needing to change it again.

[Bob La Londe]

I ditched the ATC added some spring washers to the PDB, lubed them up (appropriately), and cranked down the draw bar until it dragged to release a tool. Then I backed it off a 1/4 turn. Tool holders fall out, but not by much. Right now I am about half an hour into roughing some 4140HT with a 1/2" Accupro AlTiN coated endmill and there is no sign of tool holder walk out. During the profile cuts and in heavier cuts with more Y axis travel you can hear some chatter, but its not pulling the tool holder out.

[SCzEngrgGroup]

Bob,

I'm curious what your RPM, DOC, WOC and Feed are?

Regards,
Ray L.

[Bob La Londe]

I thought I was using pretty conservative settings. I notice the Tormach exhibits a symptom I have seen on other mills. Its more prone to chatter when traveling more in Y than in X. I was using an imperfect mill because I didn't have any good 1/2" end mills for steel. Sides were good, but the end was not perfect. 1/2" was at 1000 RPM and 1/4" was at 2000 RPM. I think surface speeds were pretty low at around 120-130 SFM. I was running all in high speed. I probably should have shifted to low for this job. Most cuts were at 1/4 DOC. I tried not to exceed 20% stepover.

Another thing I noticed with the 1/4". It liked slotting and ramping better than trochoidal material removal. It tended to chatter with the DOC side cutting loads even though they were quite light. Even spiral interpolation (basically helical slotting) chattered less. I noticed that in aluminum too a while back. Roughing some mold cavities it would plunge and rip the first path surprisingly quietly then at the same speed and much less WOC it would start to get noisy.

I did have to give the 1/2" holder a light tap with the vise handle to release once. This was a sort of emergency part to make a specialty drill guide so I could finish a mold that's too tall to fit under the head of any of my mills. I could have made it out of aluminum, but I wanted to make it out of steel so it would last longer. I have 4140HT left over from another job. Aluminum drill guides tend to get wallowed out fairly quickly. If you are interested I wrote up the reason for the drill guide here: Drilling and Pinning Hinged Molds Yeah I know a steel drill guide can dull drill flutes, but you really cut with the tip, and by the time the part is ready to have the hinges drilled and pinned Its worth a lot more than a drill bit.

I have to say the Tormach really doesn't like 4140HT. Surface finishes were not at all like I have gotten on my other machines. I suspect its just not rigid enough, although (with a radically different feed/speed/load process) the Little Speedmasters do ok. Either that, or I just haven't found the sweet spots on this machine yet. I watched some of the "steel" cutting videos on-line and the first thing I noted is that many of them do not say what kind of steel. There are one or two that say they are cutting 4140, but I am sure it must be in the annealed state. There is a good value to be able to cut 4140HT if 28-32 is enough hardness for the job. No having to send it out for heat treat over sized and then having to grind to final dimension.

Today I need to deck off the back of my jig and drill it. Probably be the last time I run 4140HT on the Tormach for a while unless I get a custom job that calls for it.

P.S. I was not all that pleased with the Superfly for the 4140HT either. I tried faster speeds and feeds, but wound up dropping to 250rpm and 1.88ipm at 40%woc. It was serviceable, but not at all like the finish I would have expected. I damaged one insert point at higher speeds. I'll have to look at the one that is currently down and see if it survived the job. Yes, with the "steel" insert.

P.P.S. I can see why some guys say buy mills with the shortest flutes possible. You can't use them anyway. LOL.

[Steve Seebold]

Before I bought my 1100, I considered a 770 because of the 10K RPM spindle. Then I did a little more reading ant I learned the 770 only had 1 horsepower. My 1100 has 1.5 horsepower but it only has a 5140 RPM spindle. I have no complaints with the 5140 RPM spindle. I can still do anything you could do on a high dollar machine, it just takes me a little longer.

[Bob La Londe]

Before I bought my 1100, I considered a 770 because of the 10K RPM spindle. Then I did a little more reading ant I learned the 770 only had 1 horsepower. My 1100 has 1.5 horsepower but it only has a 5140 RPM spindle. I have no complaints with the 5140 RPM spindle. I can still do anything you could do on a high dollar machine, it just takes me a

little

longer.

I bought my 1100 as a stop gap machine between my 3600rpm 4HP rate (5hp motor) Hurco KMB1 and my 24,000 RPM 2HP Speedmasters. A "liitle" slower is right. LOL. Its not really rigid enough or powerful enough for hard steel machining or fast enough for aluminum machining, but it does them. Its very much a compromise machine. High dollar is a very misleading comparison. You rig a Tormac 1100 out like a VMC and its only about 6 grand less than a Haas Mini Mill. Trust me I wish had bought the Haas, but to be honest the other Haas machines I had looked at where to much further out of my price range. I didn't realize they had a machine in my budget range until after I bought the 1100.

I make my posts about what I can do and to honestly help others. I may not always be right, but I try not to mislead. Saying a Tormach 1100 can do anything from aluminum to titanium is true, but you can say the same thing about a Taig. I know. I pushed my Taig far further than it was ever designed for.

[Bob La Londe]

While paying jobs were running on the Speedmasters today I made some vise handles for the smaller mills vises I own. I made a few for the larger vises a couple days ago, and gave one to a good friend who does manual machining in his shop only to find out it was to big for his vise. He gave me the measurements off his 5" mill vise and its about the same as my 4 inch vises, I threw on a piece of 3/4 inch aluminum flat bar on the mill, modified my CAM file, and nested the job to make five of them.

Anyway, when I setup the job I swapped the Super FLy back to an aluminum insert (and reset the height). When I pulled the steel cutting insert off I saw that the tooth I had been running at 250 rpm and 1.88ipm was just fine.

[Bob La Londe]

I suppose I should add that the steel cutting inserts "look" round on the edge, and is my first thought why I was disappointed with surface finish. 4140HT likes to be CUT not rubbed. Maybe I'll grab one of each type and look at them under the magnifier lamp when I have a spare minute.

[popspipes]

Thats what they call burnishing the edge, makes the carbide resist chipping better when cutting steel, or other hard materials.

[Bob La Londe]

Thats what they call burnishing the edge, makes the carbide resist chipping better when cutting steel, or other hard materials.

Might be ok with a non work hardening steel.