[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.