CNC Equipment and Tooling recommendations

[Mark_B_4545]

Our team has recently acquired some new sponsors (finally!) and they've donated us some CNC equipment and money. It's a Tormach PCNC 1100. We're happy to accept the CNC, but we're not very experienced with it. I have some experience with machining, but that was a long time ago, before CNC machines were common.

Basically, I'm looking for a bit of advice as I wasn't prepared for this, and I have to make some decisions kind of quickly. If anybody has positive or negative experience with the machine (or CNC with FRC in general), please let me know. I'm hoping the tormach will work for us. I HAVE read the previous posts about CNC tooling from Cory, which were very informative.

We're in a bit of a weird situation so we were wondering if anybody had suggestions for how to use the money- we have a CNC mill, but we don't have a normal mill. We do have access to a lathe, and we're happy with that.

What I'd like to do is take a local class on CAM software (I'm thinking MasterCAM, I have some very basic experience...any suggestions?) and spend money on tooling. I've seen the threads on here, and I've got a preliminary list.

T-Slot hold down kit (purchase)
2 nice Kurt vises (given to us)
Coolant (what type??)
Drill chuck for R8
Collet set(.125, .250, .375, .500, .625) sizes

Endmills:
We've been given some spare tooling, but most of it is weird stuff. We've got lots of tiny (<.125") end mills, and some huge stuff, but nothing great. It's mostly carbide stuff.

I'd like to purchase some of the HSS two sided end mills (for when we break them..) from McMaster- just the normal stuff (.125, .250, .375).

We've got the 4th axis, so we're likely to try doing some gear making with involute gear cutters, but we may wait on this purchase for a bit.

It came with a 6" diameter face mill, which may be a bit big. I don't see us having to do too many face milling operations, so I'll probably hold off on purchasing for a while.

I'll also get an edge finder (did you know they make ones that make noise?) and a dial test indicator (the one where the needle rotates instead of going in and out). Has anybody had experience with McMaster's "economy" indicators? They're a lot cheaper than the Brown and Sharpe.... I don't want to get one if it's like their "economy" calipers, which were the worst (Grizzly IIRC) calipers I'd ever seen. I get suspicious of things like this.

Is this enough for our first year? Our most ambitious plans would include at most doing gearbox plates, multi sized hex shafts on the 4th axis (how do you program this?), putting some lightening/locating features in some thin walled rectangular tube, maybe some type of wheel/roller, pulleys or sprockets, and lightening patterns in steel gears.

My goal is to not spend a bunch on tooling, so if anybody knows places to get this sort of stuff cheap, it would be appreciated.

This may be a really, really dumb question, but if we'd like to save money and not get a probe style indicator, can we just zero the z axis by slowly lowering until we can't slip something thin underneath, then take off the thickness of the thin piece?

My second question deals with the Tormach. What can we cut and how accurately can we do it? The machine looks good, but I am clueless as to what can actually be cut at reasonable speeds. I've been doing some math, and to me, it looks like the limiting factor will be spindle RPM (5100 or 4400 rpm-does anybody know which is correct) for using the .250 endmill. I'm getting values of over 20 inches/min with a .125 deep cut, which seems like a lot, as I'm visualizing trying to do that on a smaller mill. How rigid is the tormach? I think I'll buy GWizard to do the math for me. I'd like to try sprockets (steel and aluminum) eventually. Is this feasible? Also, how accurate can we get a circular hole? I'd love to be able to do bearing bores without needed a reamer.

[Gray Adams]

Go with the TTS - Tormach Tooling System. If you use their holders, its way easier to run through tool changes. Sure its a bit pricier, but its really nice to be able to run a program with 5 tools and not have to stop and Z0 the tool each time. You could probably get some used holders off ebay or something. 2 drill chucks, a bunch of endmill holders, a 2.5" or so facemill.

You can get away with most of your machining with a .250" endmill. HSS is good for aluminum, its a lot less rigid (i.e. breakable) than carbide. You'll need some larger some smaller cutters, but in general, go with either .250", .5" if it needs to be bigger, or any smaller size as needed. .250" is a good workhorse for FRC sized stuff.

I can't say much about coolant, but I could probably ask some guys on Monday about what we use at work.

An edge finder would be good, but if you really don't want to spend the money, stick a nicely ground .500" pin in a collet or drill chuck, push your piece up against the pin, and call that zero. A DTI is pretty essential for relocating parts around anything ciruclar (holes or bosses), so I would go for one. McMaster should be ok, just don't expect it to put up with abuse or last a long time. But its a good place to start until you really understand what you need.

For Z0ing, that's exactly what a lot of people do - try to slide something between the tool and the workpiece until it no longer fits. Your trusty .500" ground pin is good for this, as is a 1-2-3 block or anything else that you know is a very precise size.

As far as CAM software goes, I've had great experiences with HSMXpress. It's free for solidworks, and Autodesk owns it so I can only imagine you can get it for Inventor. MasterCAM is great, but might be overkill if you can't get it super cheap.

I would stay away form the 4th axis for now until you get to know your tools and machine. It's rare that you'll need it. If you want to do cool stuff with making hex, there's always these (http://www.mcmaster.com/#collet-blocks/=t442a5) used with a vice.

A PCNC 1100 isn't super powerful or rigid, so I would stick to shallower cuts, on the order of maybe .040" to .050". I've always been conservative with my cutting since I usually don't make more than half a dozen or so of any given part. 2 or 3 shallow cuts is way better than 1 deep cut at 1/3 of the feed. I've never been able to get G-wizard to give me good numbers on a Tormach, it just doesn't have the coolant flow or rigidity needed to get those numbers. Stick to .050" deep, and adjust your cutting feed as necessary to not break tools/give a good finish.

Other things: Get a 90 degree spot drill bit. I use them all the time for spot drilling, chamfering, and occasionally countersinking. If you can spot drill and pre-chamfer a hole at the same time and then break all your edges with the machine at the end of the program, your parts are way nicer and come out faster.

Build a small tool library of stuff that always stays in the holder. Set the heights once, never worry about them again. I mean, how many tools do you really need? A spot drill, a few end mills, a face mill, and a few drill bits (these change often though).

My workflow on the PCNC 1100 was usually take oversize stock. face mill a bit off the top, machine the part almost complete with .125" or so stock on the bottom, clamped in the vice, flip the part over and clamp the finished edges in the vice, and run the facemill to cut off that .125" extra. It works for most parts, it keeps all or most of your features done in the same setup, and you don't leave any stock surfaces.

[Chadfrom308]

Congrats on the CNC machines! I work at a CNC machine shop (Precision Karting) and they are the best and worse machines ever. They can be really useful if you know how to use them and they can be a pain if you crash them.

First thing first. turn the rapid down. It is worth waiting a not crashing the machine than going quickly. The rapid is how fast it moves from position to position without cutting. Turn that down until you ran a program and it works 100% (our CNC lathe from Haas is locked at 50% rapid max)

And Carbide tools are better than HSS, but they will chip and break so much easier than HSS. If you touch the tools off wrong, then you can break them (I've done that a couple of times). Most of the time you can get them resharpened for cheap.

So when you make a program, you build your holes and contours around a work offset. When you put material into the machine, you have to set the work offset. If you have edge detectors, the easiest way is to program the work offset to a corner of the material.

I am not sure how the Tormach works, but if it is anything like a fadal or haas, what you have to do is put it into hand jog mode and jog near the corner. Turn it down to .001" and then slowly go until you hit the edge and then set that work offset (g54).

Next thing you have to do is touch off the tools. Get a thin shim, (we use .006" shim) and go down and touch the cutter to the shim (slowly, especially with carbide). If you get it down to about 1/4" off the material, then turn it down to .001" per click of the jog handle, then jiggle the shim and lower the tool down till it pinches the shim and you cant jiggle it anymore, that is the easiest method. (thats what we do) (and probes are only really for setting work offsets and tools. If you get a fancy system, you can set tool offsets by using a tool probe (which you still need to touch off 1 tool))


The speeds and feeds are a little weird and change with every tool. Carbide cuts more and faster and HSS cuts slower but is more forgiving. I would try to get ahold of some insertable tools. If you break and edge, you can normally rotate the insert a couple of times instead of buying a whole new tool. ISCAR makes really good stuff, but it's also top of the line and expensive. (they might help you out, they are pretty nice)

The easiest thing to do is to just look the tool up online or call whoever makes the tool and ask them, or get a reference sheet. And since you guys aren't doing any high-volume manufacturing, try to use the minimum speeds and feeds.

I wouldn't use the 4th axis until you are really comfortable with the machine.
I dont even know how to program it

If the machine comes with coolant, thats great. If not, then you can use WD-40 unless you are doing some serious cutting (like fast and deep cuts)

I am not positive how accurate tormachs are, but most CNC machines can go to .001" which is probably good enough for anything FRC. Tormachs are really low powered, but most things will be fine with it. Circles should be fine as well.

Any other questions? I think I answered most of them. That's just what I have learned (which is basic). Feel free anyone else to correct me and give more advice.

[Cory]

Setting Z offset is much safer if you use a ground pin (.250 and up works great), jog the tool to a height above the part that the pin will NOT fit under, and then attempt to slide the pin under the tool with gentle pressure as you slowly jog the tool up by .001 at a time until the pin can slide under the tool either freely or with light resistance.

You eliminate (almost) any chance of chipping the tool by jogging it into your pin/shim/part, since you are going up instead of down. If you were to jog the wrong way, you have a pin diameter's worth of buffer zone before you hit anything.

[Mk.32]

Originally Posted by Gray Adams

A PCNC 1100 isn't super powerful or rigid, so I would stick to shallower cuts, on the order of maybe .040" to .050". I've always been conservative with my cutting since I usually don't make more than half a dozen or so of any given part. 2 or 3 shallow cuts is way better than 1 deep cut at 1/3 of the feed. I've never been able to get G-wizard to give me good numbers on a Tormach, it just doesn't have the coolant flow or rigidity needed to get those numbers. Stick to .050" deep, and adjust your cutting feed as necessary to not break tools/give a good finish.

The tormach is decently powerful and rigid... imho I run one at the makerspace and for the team:

This is just an example of what is possible with the right tooling. https://www.youtube.com/watch?v=TVEERG0mBzU
I've had good luck with GWiz but it takes some tunng to get to run right. Personally with my 1/4 2 flute tools .1-.15 DOC is not a problem.

The basic advice I can give for setting up something like this is, start small and buy tools as you need them and then it's highly recommended you have an "expert" around to help you setup and get comfortable running the machine. the TTS is a good way to go, the basic kits should hold you over with most of the tool holders you need. I also would not buy tools from McMaster-Carr due to pricing.

Also Cory from 254 has some really good posts about tooling setups if you dig into his post history a little.

[DampRobot]

Originally Posted by Cory

Setting Z offset is much safer if you use a ground pin (.250 and up works great), jog the tool to a height above the part that the pin will NOT fit under, and then attempt to slide the pin under the tool with gentle pressure as you slowly jog the tool up by .001 at a time until the pin can slide under the tool either freely or with light resistance.

You eliminate (almost) any chance of chipping the tool by jogging it into your pin/shim/part, since you are going up instead of down. If you were to jog the wrong way, you have a pin diameter's worth of buffer zone before you hit anything.

Seconded. This method is much safer for your tooling than trying to slide a piece of paper under the tool, and is also much faster (as overshoot is much less of an issue, and it's fast to check height by sliding something underneath). I usually use a 1-2-3 block, but it's honestly whatever you prefer/have lying around.

Originally Posted by Mk.32

The tormach is decently powerful and rigid... imho I run one at the makerspace and for the team:

This is just an example of what is possible with the right tooling. https://www.youtube.com/watch?v=TVEERG0mBzU
I've had good luck with GWiz but it takes some tunng to get to run right. Personally with my 1/4 2 flute tools .1-.15 DOC is not a problem.

I'll also attest that Tormachs are really pretty sweet little machines. Sure, they might not measure up to a HAAS, but they're great entry mill. I also ran one at a local hackerspace (TechShop) and was impressed.

I had no problem running 1/4" 2 flute mills (I beleive ZrN coated) with 3/16" passes in 6061 alu and flood coolant. If I'm remembering correctly, I could get 20 IPM at 4000 rmp without any vibration issues.

You should be able to get press fits out of the Tormach, but it will take some trial and error. Don't expect a 1.125" roughing pass to give you a nice press fit, realistically you're going to have to do something like step down at 1.105" diameter roughing and then do a finish pass at 1.125" diameter (or slightly over, if that's what you find works better). With careful milling and freshman with sandpaper just in case fits don't come out right, we've never needed a reamer.

Another thing: you're going to want to do some research on how FRC teams like to do mill fixtures. Clamping with toe clamps is an enormous PITA, especially if you have to move them every three seconds because you're profiling.

In terms of tooling, I'd get a full number and fractional drill set, extra drills for the sizes you've standardised with (for example, we got extra #7s for #10 screw clearance, #10s for 3/16" rivet clearance, and #21 IIRC for 10-32 tap drill), 3-5 1/4" 2 flute aluminium endmills, 2 or so 1/2" endmills, and maybe a few 1/8" endmills for good measure. A set of parallels can be useful as well.

Get the Tormach Tooling System. It's easy to use, the standard for Tormachs, and plays nice with toolchanges in Mach 3 (the Tormach software).

One last thing, not necessarily related to milling, but a 1/2" hex broach can be an amazingly useful investment. Just something to think about as you're investing in tooling.

[Mk.32]

Originally Posted by DampRobot

One last thing, not necessarily related to milling, but a 1/2" hex broach can be an amazingly useful investment. Just something to think about as you're investing in tooling.

Agreed, (milling out Hex with knocked out corners is possible) but having the broach sets for hex/keys/etc is very useful.

And just in case OP is not experienced with broaching... do NOT use the Tormach for any kinda of broaching. A press or LARGE lathe is much better suited.

[Jared]

We have a Tormach PCNC 1100, and we really like it.
Here’s some info from one of my previous posts:
It may not be the most rigid, most powerful CNC machine, but it’s in a different price range from the nicer Haas mills. Overall, the Tormach is a pretty decent setup. The Mach 3 software (CNC controller) is very nice and makes it very easy to use. We don’t have any mentors with serious CNC experience, but we do have a machinist, who helps us with making decisions on end mills/materials. Apart from that, the machine is really easy to use and doesn’t require tons of experience. We have a handful of students who can do everything on the machine by themselves, and they haven’t used it for that long.

The tormach’s biggest drawback is probably the computer that runs Mach 3. It wants to be an old, simple, machine with few drivers and Windows XP, with a specific service pack (IIRC, it’s SP2). Even then, when the display goes to sleep, the spindle speed starts oscillating, or when somebody is welding, things start moving by themselves due to electrical interference. Turn off power when it’s not in use! The steppers that drive the axes can slip under high acceleration, such as moving the table with keyboard keys, or e-stopping the machine. I’ve broken several bits because the machine’s zero position changed after I stopped it.

There are two (or more?) hardware revisions of the Tormach 1100. Our old one, which was water damaged, was the older revision, which has a slower 4400 rpm spindle and inferior motor drives. The new one has a faster 5100 rpm spindle, as well as a few changes to the oiler, front control panel, and some newer handles/latches. The new one’s oiler is also higher up which I think is an attempt to fix the lubrication issues with the z axis. The older one’s z-axis sometimes freefalls during a tool change or a reference program, which is very terrifying. This could be an issue with just our Tormach.
As for CAM software, MasterCAM has very good toolpath generation, but can be difficult to use. We use X4 with no maintenance updates, which is from 2008 and slightly buggy, so it may have gotten better over the years. Its user interface is incredibly unfriendly for beginning users, and the whole concept of work coordinate systems and construction/tool planes can get confusing for 4 axis work, but if you spend some time with the program, you can figure it out. Getting the post processor (which converts toolpaths to machine readable Gcode) can be a challenge. One of MasterCAM’s built in posts works, Mach 3 has two different post processors you can add, and Tormach has a post processor you can add. Tormach’s post processor, which is a modified for machine limits version of a random internet user named creep_pea’s post processor for Mach 3, seems to be the best, only having issues with peck drilling operations. For 4th axis simultaneous work (rotating the part as you cut, vs indexing to machine on a plane), Mach 3’s company created post works differently from the others.

For zeroing the z-axis, we do something similar to what you describe, but you need to be really careful to not damage the end mill. As we slide a piece of paper back and forth on the surface of the part, we lower the end mill one ten thousandth at a time until the paper no longer moves. We don’t bother subtracting the thickness of the paper, and depth ends up within .003, which is good enough for almost everything we do. Make sure your part is held down well for this. It likes to bend and warp when clamped poorly and after cuts, so it can be helpful to use a surface you know is flat to make sure your hold downs aren’t warping the part.

The tormach is actually quite accurate. We can hold +/- 0.0003” on circular features. It’s easier to get within .001”, which is adequate for a bearing. You will need to tell MasterCAM the exact diameter of the cutting tool to get this accurate, which can be a challenge, as calipers don’t fit nicely over 3 flute end mills. You can mill a slot and measure that instead. We’ve had our best experience taking a full depth finish cut .015” wide at 10 IPM with flood coolant and a McMaster Carr HSS .250 flat end mill with 3 flutes.
Personally, I’ve never had a problem with spindle rpm being too slow. In general, I usually run it at 5000 rpm in aluminum, and 1500-3000 in steel, depending on the bit. It’s definitely too slow to make good use of carbide bits though. We have GWizard, and it is very nice, but can sometimes be a little optimistic about feeds. I really recommend starting slow and working your way up. As soon as it starts to chatter, your surface finish gets worse, and your tools break quickly.

For coolant, we use Mobilcut 102. It works well as both a cutting fluid and as a way to move chips out of the way. If you end up going through already cut chips, you’ll break a bit, so I recommend using a decent amount of pressure with the coolant. We put ¾ of a cup full of the oil into a gallon of water. It does evaporate and magically disappear, so be sure to buy plenty. Also, it’s a good idea to flush/clean the coolant system every now and then so it doesn’t smell like a dead animal.

For lubrication of the ways, it’s important to fill the oiler with way oil (we use mobil vactra 2) and give it a pull every time you use the machine and run all the axes back and forth a few times.

If you plan on using it a lot, there’s an automatic tool changer and power drawbar you can get. The power drawbar is really nice for quick tool changes, but we had to take a flap grinder to the motor mount to get it to fit correctly. If you’re taking an aggressive cut, and you haven’t tightened the drawbar enough, then the tools can get pulled out. It’s easy to forget sometimes… Also, you don’t have to worry about people hammering on the drawbar when the threads aren’t engaged.

If you have any more questions, let us know.

[Gray Adams]

Originally Posted by Jared

The tormach is actually quite accurate. We can hold +/- 0.0003” on circular features. It’s easier to get within .001”, which is adequate for a bearing.

That sounds absurdly tight for helical interpolation on anything but the higher class Japanese machines. How are you even measuring that kind of tolerance? Even if you could hold that kind of tolerance, with the thermal expansion of aluminum, holding a part with a 1.250" hole in it in your hand for a few minutes will cause the diameter to grow .00033 in.

Anything even close to that tight should be done with a boring head or reamer anyway.

[Jared]

Originally Posted by Gray Adams

That sounds absurdly tight for helical interpolation on anything but the higher class Japanese machines. How are you even measuring that kind of tolerance? Even if you could hold that kind of tolerance, with the thermal expansion of aluminum, holding a part with a 1.250" hole in it in your hand for a few minutes will cause the diameter to grow .00033 in.

Anything even close to that tight should be done with a boring head or reamer anyway.

We measured on a CMM. Here are the results, listed as nominal, measured
1.1250, 1.1249
1.1245, 1.1250 (our first try, incorrect cutter comp)
0.8750, 0.8747

I did the math for how much temperature affects diameter, and for a 1.125" hole, it was around 20 degrees F to get a change of .0003. It's likely there wasn't a 20 degree change, as the machine's coolant is at room temperature, the part was machined at room temperature, the bearings were installed at room temperature, and the measuring was done at room temperature.

[Mark_B_4545]

Wow! Thanks for all the info, this is great.

Gary: What about the Tormach Tooling Setup makes it so you don't have to zero the Z-axis each time? From what I've learned on MasterCAM so far, you can tell it which tool you're using, and program an offset for the tool. I think I agree about the .250" end mills. As for the 4th axis- I agree, it doesn't seem super useful, but we got it for free, so I at least plan to check it out sometime. As for coolant flow you mentioned, I don't think it should be a problem. They've installed their own pump instead of the factory one. I like your idea with the oversized stock. I was just planning to use tabs and cut them out.

Chad: Good advice on the rapids. I hope to take it slow and not break anything on our new machine. For the tools, I'm getting a few of McMaster's double sided end mills in case anything goes wrong.

Cory: Great idea for zeroing the z-axis. We'll do this for sure to avoid crashing the tool into the part.

Mk 32: That's a great example! It seems more rigid than I expected. I've done some research, and I've seen plenty of people go with some deeper but slower cuts, like your .1 to .15 DOC. I agree that McMaster is a bit expensive, but they have some stuff our local supplier doesn't have. We try to buy at our cheaper local place as much as possible, but they don't have everything.

Damprobot: Good suggestion about the hex broach. We might not have the best press for it though, so I think we'll wait, try doing hexes on the CNC, and if that's too much of a pain, we'll by a press/broach.

[Gray Adams]

Originally Posted by Jared

We measured on a CMM. Here are the results, listed as nominal, measured
1.1250, 1.1249
1.1245, 1.1250 (our first try, incorrect cutter comp)
0.8750, 0.8747

I did the math for how much temperature affects diameter, and for a 1.125" hole, it was around 20 degrees F to get a change of .0003. It's likely there wasn't a 20 degree change, as the machine's coolant is at room temperature, the part was machined at room temperature, the bearings were installed at room temperature, and the measuring was done at room temperature.

Well, machining is rarely at room temperature. If it was you wouldn't really need coolant (yes I know that coolant primarily carries chips away).

But that's really impressive that you got such high precision on a machine like a Tormach with an endmill measured with calipers. The PCNC 1100 is not that precise of a machine though, and the only way you can achieve those numbers is with repeated adjustment to dial it in. The inspection sheet for this machine allows for .00118" of spindle runout alone, the axis repeatability is specced at .00078". I don't disbelieve that you got the numbers that you did, but it certainly shouldn't be expected behavior from a machine like this and a dimension like that should take numerous attempts to dial the machine in. I wouldn't think twice if you told me you got that from an Okuma or Mori Seiki.

Originally Posted by Mark_B_4545

Wow! Thanks for all the info, this is great.

Gary: What about the Tormach Tooling Setup makes it so you don't have to zero the Z-axis each time? From what I've learned on MasterCAM so far, you can tell it which tool you're using, and program an offset for the tool. I think I agree about the .250" end mills. As for the 4th axis- I agree, it doesn't seem super useful, but we got it for free, so I at least plan to check it out sometime. As for coolant flow you mentioned, I don't think it should be a problem. They've installed their own pump instead of the factory one. I like your idea with the oversized stock. I was just planning to use tabs and cut them out.

The holders have a straight shank that slides into a 3/4" collet and ring on the outside of them that sits nice and flush with part of the spindle. Its always the same length tool as long as you don't remove the cutter from the holder. You measure it once, set the offset, and then call up that offset every time you use the tool. This is part of why you should have a tool library of tools that never leave their holders.

If you have an upgraded pump that should help a lot. The one I used to work on needed to be basically full of coolant and even then the pressure was low. If your tank started to run down due to evaporation, coolant flow would be horrendous.

[DonRotolo]

All the advice above is good, just consider that you actually have two "problems" to solve:

The first, and most obvious "problem" is learning how to use CNC stuff. You can design things in Inventor or Solidworks, then use a program like MasterCam (which might be a little overkill) to convert the design into G-Code which is what the Tormach controller uses to actually move the machine axes.

The second, and more subtle "problem" is learning how to use a mill. Break this into a few pieces:

Speeds and feeds: There's a lot on the web about this, so the short version is that for every given cutter and material there is an optimal rotating speed, feed rate and depth of cut. Too slow and you wear the bit almost instantly, too fast and the bit breaks.

Cutting tools: Buy a set of 'many' sizes until you get a feel for what you use most. Don't get TiN coated bits for aluminum - these are great for steel but aluminum wants to stick to it, which is bad. Look at McMaster 88505A35 or even better at use-enco 320-0006. McMaster is very expensive and has a poor selection of tooling. Really small tooling is only useful in special situations.

Design for manufacture: The part needs to be able to be made. Not everything can.

Care and feeding: You need to understand the maintenance and care of a mill, and be absolutely crazy about making sure its being done all the time and correctly. That machine is NOT inexpensive, likely 10 times the cost of the lathe, about as much as a small car. Treat it right and be absolutely intolerant of anything else.

All that being said: Get in touch with Tormach. They really have a great program to get you started and answer all your questions. Use them as a resource, you'll be very pleased you did.

Also, this is an opportunity to reward those 'best' students: You can't train everyone to run the machine, so hold it as a 'reward' for <something>.

[Jared]

Originally Posted by Gray Adams

Well, machining is rarely at room temperature. If it was you wouldn't really need coolant (yes I know that coolant primarily carries chips away).

But that's really impressive that you got such high precision on a machine like a Tormach with an endmill measured with calipers. The PCNC 1100 is not that precise of a machine though, and the only way you can achieve those numbers is with repeated adjustment to dial it in. The inspection sheet for this machine allows for .00118" of spindle runout alone, the axis repeatability is specced at .00078". I don't disbelieve that you got the numbers that you did, but it certainly shouldn't be expected behavior from a machine like this and a dimension like that should take numerous attempts to dial the machine in. I wouldn't think twice if you told me you got that from an Okuma or Mori Seiki.

If you have an upgraded pump that should help a lot. The one I used to work on needed to be basically full of coolant and even then the pressure was low. If your tank started to run down due to evaporation, coolant flow would be horrendous.

Getting within a thousandth did require multiple tries and was a time consuming process which we did because we couldn't find the reamer, and is not typical normal operation, but is possible if you try really hard. We measured a slot the end mill cut with calipers, then made 5 tool paths, that were +/- .0002", measured these holes, then picked the one that appeared closest to the correct diameter. We have an end mill we use just for cutting finish passes so we don't wear it down. We can get very repeatable results, but it's difficult to get the number you want (very precise, low accuracy).

The installed coolant pump is a disaster. It's a made in China pump, complete with labeling/specs in Chinese. Be sure to keep filters in place for the pump. We dealt with coolant shortage the whole season, and the pump just doesn't run when there's less than 5 gallons in the tank, and if the tank is less than 75% full, the pressure is awful.

The Tormach Tooling system is very cool and will always get pulled in all the way to the machine. I do not recommend the set screw holders. Your tools will get sucked out of the holder if you make an aggressive cut. If possible, label tools in your tool libraries. People have a tendency to adjust stickout for a particular task without telling you.

[Cory]

Originally Posted by Gray Adams

I don't disbelieve that you got the numbers that you did, but it certainly shouldn't be expected behavior from a machine like this and a dimension like that should take numerous attempts to dial the machine in. I wouldn't think twice if you told me you got that from an Okuma or Mori Seiki.

It's not clear whether those CMM values were for one part each or for a run of parts...but I would be absolutely shocked if you could consistently (without constantly chasing offsets) hold .0003 on a run of parts on a Tormach.