If your company was profitable last year, purchasing would be a better way to go. You can depreciate most of the machine on the first year's taxes (still paying the same amount, but you have a machine for the $$ vs giving it to the gov) You can get a $1 buy out lease quite easily, but you are pretty much buying the machine like above.

The PH Horn broaching tools work quite well. Havn't used them on a VMC, but have on a couple of parts on a 2 axis lathe and they hold up quite well and are very consistant (but you pay for it too)

About 80% of our work is hardmilling in Ramax, Mirrax, S-7, A2 and D2. S-7 would be the best bet IMO. As far as tooling, we have tried ALLOT of brands (Haneda, Frasia, SGS, ISI, Union Tool, etc...) and we have the best bet with Seco/Jabra endmills. For a .030 ball, try Seco's "113" series ballnose, we would use the Seco# 113ML008TN (.8mm ball), with only 8000 RPM though you will be down in the 12-13IMP for finishing though.

Im not saying its the best machine out there, it isnt. Never said it was. But, with an open mind one can get creative. And we sell many other lines of lathes (The other Haas SL lathes, Hyundai, and Nakamora) and for what the customer needed we could sell them 5 spindles for the cost of one. I am fully aware you cant do 1 ton work with a 1/2 ton pickup, but sometimes you are just throwing profits and productivity out the window to do 1/2 ton work with a 1 ton truc.

You would have to see the application. Not every part out there has 1" of material on the face and OD that needs cut off of the part. The size of the part and the tooling fell well in the envelope of the TL's speed and feed. These would be the speed and feed on any machine. Put at it this way, if you have purchased a ATV if the last 2 years or so, this customer manufactures about 70% of the OEM half-shaft dirve shafts for the US built ATV Market (Honda, Cat, Polaris, Kawasaki and Yamaha) and has a whole shop full of Okuma LU and LT turning centers (30+ machines) and these lil' ol TL's do a damn good job of what they were intended to do. Given the situation, the TL can run this part 60% faster, using the same speeds and feeds, than they were previously on their Okumas. Even with a robot it took well over 10 seconds a piece to load the part in and load another 10 to get the part out of the machine working around the sheet metal, tailstock, turret and door. With the TL there was no door to work around, and the gang tooling allowed us to setup 3 tools with no tool changed time. less than .5 second chip to chip.

Haas lathes don't have a prox switch on the chuck, so they never know if the chuck is closed or not anyways. It just watches the sequencing of the footpetal switch basically. Turn Off #278 and see if you get "Chuck Open" message on the machine while you cycle the chuck. If it does, then the machine won't start when it "thinks" the chuck is open anyways.

For the record, the code for programming is the same as the other Haas lathes, code for code, line by line. And that code would run 90% of your Fanuc Control 2-axis lathes on the market without much if any changes.

Leigh - The proge is well worth it, ans so you know you can use full Renishaw Macros with it also, you are not just limited to Haas's macros. DO NOT GET THE MARPOSS probe package, spend the extra $500 for the Renishaw, the software on the Marposs still has allot of bugs in it. TL-4, that thing is a BIG lathe (8" thru hole and I think 1500 ft lbs of torque, and other than a Okuma LOC-1 (Lathe-Oil Country) you are looking at something custom built for big parts.

For secondary ops (drill / spot / chamfer etc) where a robot or automation was used we setup a TL with air chuck and a custom built gang tool plate. The part only needed about 700 RPM, and with the we could spot / drill / tap the part quicker since we had no tool changes.

MC X4 will do a fine job on the TL I have used it quite a bit with a good Haas Lathe post (that is the key, getting your MC dealer to get you a good post for a HAAS lathe and it's specific G-Code) It's unfortunate that your local HFO isn't getting the job done with the training. I spent 3 years doing Haas training for one of the larger HFO's in the country, and in 3 days of training (One TL Lathe Operator 1 day class and one 2-day Haas Turning center programming class) and you can pretty much cover the basics of "Real World" machining on a TL Lathe. The capability of the TL is it is a 2 axis turning center without a turret. 80% of the parts you can do on that machine could be programmed on the machine. Turning centers have a series of nice canned cycles that can cover just about every Type I roughing part out there. If doing Type II roughing (candlestick holder looking parts, or dumb-bell looking parts) then MC can be a real help. And oh yea, don't let the TL fool you, I have set up a few that can out produce turning centers at 5x the cost. YOU CAN do live tooling with it (just need a air or electirc driven tool) and using gang tooling you can make parts faster than a turrett (no cycle time wasted when changing tools with gang tooling)

gUNTHER - Do you have any documentation (english) for using the xss or css features?

Gunther, X+ is a great program, thanks for working on it! All I have issues with are the "TEMP files. We use multiple setup sheets for each .mcx, and store these setup sheets in the same folder as the .mcx If I make 2 setup sheets ( one for the top of a part, another for the bottom ) the 2nd setup sheet will overwrite the "TEMP" image that is stored in the destination folder for out File Setup in the .mcx file. What happens is this will overwite any images in our earlier setup sheets in that folder. Any way to work around it?

With the new X+ setup sheet, why dont we share some sample .xss files and see what works good for others.

I too see this. We use multiple setup sheet for every .mcx file, and try to store these setup sheets in the same folder as the .mcx on our network. The .hml files reference the .png file "TEMP", and the"TEMP" is created and overwitten eveytime you create a new setup sheet, it overwrites the images in any older setup sheets in that folder. I am still working on how to work around this in my shop.

BULLETBOB - I DONT REALLY THINK YOUWILL LOOSE A WHOLE LOT OF ACCURACY UNTIL YOU START GETTING TO THE LIMITS OF THE SPEED OF THE TRUNION, BUT YOU WILL REACH A POINT WHERE CHANGING THE PARAMATERS WILL NOT GET YOU MUCH MORE SPEED, WHERE YOUR ACCURACIES WILL DICTATE HOW FAST THE PART WILL RUN. BASICALLY ALL THOSE PARAMATERS DO IS TIME HOW OFTEN THE CONTROL CHECKS ITS POSITION, MEANING EVERY 8000 ENCODER COUNTS (WHICH IS STILL CHECKING QUITE FREQUENTLY, THEY SHOULD BE 1-MILLION PULSE ENCODERS ON THE B-AXIS, MEANS 1MILLION COUNTS PER 360 / DEGREES)

Bob - I bet there is more tuning issues than anything, but that is a guess. Unfortunately the paramaters are not the easy ones to get to. If you know how to get into the Axis Paramater pages, then go to the A and B axis each, you will see them. I would get your machine sales guy envolved also, he will be the one to carry the most cout with getting the right attention.

THe 5-axis drives may be a issue (how the drives are tuned) not many HFOs have allot of knowledge of the rotary axis products. We had one guy who was real good at tuning the trunions and it would make all the difference. Its hard to diagnose over the web, but if it got faster at .001 then we may be on to something.

Take a scientific approach to it. If the cut tol is .0002, and it is working good at G187 P3 E.025, then go up on the Cut Tol to .001 for example, and see if we can go up on the E value. If the machine is "bumping" (sounds like someone is drumming on the sheetmetal) the machine is trying too hard to stay tight. Also, being it is 5 axis, and it is a cylinder head, what kind of head? Motorcycle? Car head? How close to rotation centerline are you? You might be at the limit of an angular feed max of the rotary product. The farther away from centerline the slower you can run.

The P1, P2, and P3 are more for dead sharp, 90 deg G1 to G1 type moves where as the E value could be more like a NURBS type setting. I have run up to 200IPM on 90 deg square roughing routines (pocketing) and you need to get in excess of E.05 to get the machine to start to slow down at all, meaning it is mainatining the accuracy just fine and no improvment on that particular machine, acc/dec settings, etc... with a number any lower than that. There are allot of dynamics here too. Machine size / weight is a big one. Saw customers buy a VF-6SS and load programs they were running on a VF-2SS, and have surface finish problems / longer cycle times on the 6. Even when using the same "E" value. In the same example as above, testing would show the same program, IPM, etc... and the machine would start slowing down at a E.020. Why? Table mass. The builder has to use allot lower Acc/Dec settings due to table weight and max part weight. My suugestion is to run in the air with really tight accuracy settings out of X4 and mess around with the P1-P3 and E.0001-E.2000. And i do not work for Haas, but one of the larger HFos in the coutnry.

With G187 P1 it will run the Haas with it's most aggressive acc/dec parmaters, thus making the maching jerk more if you have real tight tolerancing. The maching will try to get up to speed as quick as possible from a dead stop. Stay at the P1 and open up the tolerancing on Mastercam (don't be afraid to go as high as .02). Also, you can use the "E" value which is your deviation. It can be from E.0001 - E.2000 the higher the value, the more deviation (smoother). It doense mean you will make a bad part though. Try G187 P1 E.05 and if it still jerks, try G187 P1 E.1 The Haas control can run 1000 blocks per sec, so if the tolerancing is too might it will make really short moves. MATH FOR BPS F100. IMP = 1.6667 Inch Per Sec (100/60) If tolerancing is set to .0005, that means it will take 3333.4 blocks to move thru 1.6667 inches of material, of 3333.4 Blocks per Second, which is 3x what the control can deal with. Changing to .002 will drop that to 833 BPS. The solution, make less lines of code. Make sure Mastercam is outputting 3axis arcs, not segmented (G1) moves, a simple 90 deg arc can either be one line command, or hundreds of lines of code, depending on how the Mastercam is setup. The tighter the tolerance, the more code it outputs to move the same distance. Depending on the mfg date of the Haas (I am a Haas dealer Applications Engineer) the HSM machining option will not help a ton. You can actually turn it on as a "Trial" basisfor 200 hours to see if it helps. Talk to your local HFO about that.