Sunday, November 18, 2018

Taig to "Taigmach" Mill

I plan to continue to update this "blog" post so there will be a single place where you can go to find most of the details (or at least links to other posts in the series).

Tormach Envy

I've had a Taig CNC mill for over 10 years. This has been a really great machine and has worked well for making small injection molds. About a year ago, I upgraded it to ball screws, which has given it new life (the backlash with the lead screws was getting pretty bad). I documented that upgrade here:
However, recently I've been having a serious case of Tormach envy. I've had my eye on a PCNC 770, and now 770M mill. This provides a little larger work area than my Taig, as well as other features. But there is a huge price difference. I purchased my Taig for about $2,000 (would be about $3,000 today). Whereas the 770M is about $15,000 for what I would want. That's a huge difference.

So let's take a look at what I found so compelling about the Tormach that I don't have today with my Taig.
  • More powerful spindle
  • Spindle on/off and speed control
  • A little more Y movement
  • TTS
  • Power draw bar
  • Haimer or ITTP
  • Fogbuster
  • PathPilot
Before I got into the details, there is one major thing that kept me from buying a Tormach. We're currently in a rental house while we wait for our new house to be ready, and I don't have room for a Tormach right now. This has kept me from taking the plunge. But while talking with Kevin, another hobby CNC machinist at work, he mentioned that Tormach has had serious problems with backlash. After doing a bunch of research, I came to the conclusion that this seems to impact a very small number of machines, and seems to be a result of poorly scraped ways. You can find more in this post: Facebook Post. And also in my video below:

So after a bunch of research, I learned that there are other upgrades for the Taig for the spindle motor, the frame, and the spindle. Once I'm done with these upgrades, I'll have most of what I wanted in a Tormach, but for a lower price (less than $2,200 for the upgrades). Sounds compelling, right? Let's take a closer look.

Specs Comparison

PCNC 44010"6.25"10"
PCNC 77014"7.5"13.25"

Note: I can add a .75" extension for Y on the Taig, providing a total of 6.25" travel.

Taig: 1/4 hp
PCNC 440: 3/4 hp
PCNC 770: 1 hp
770M 1.5 hp

So in many respects, the 440 is pretty close to what I would get from upgrading my Taig. Therefore, I looked at the price of a new 440 with PathPilot and a power drawbar (but no enclose, base, TTS sets, etc. so it would be a better comparison). The total came out to $7,850.

On the other hand, the Taig upgrades (new frame, TTS spindle, power draw bar, new spindle motor) come to about $2,150. This of course, is using my existing 5019CNC mill ($3,000 today) and computer. If you factored in a cheap computer and stepper controller and you started from scratch, it would probably cost about $5,000. That's still an extra $2,800 for a 440. That's probably worth it if you just want to make chips. But if you're willing to do some work, you can get a nice machine for less money.

PCNC 440: $7,850.90

  • PCNC 440 Base Machine: $5,995
  • PathPilot Controller: $795
  • Power Drawbar: $695
  • Standard LCD monitor: $195.50
  • Keyboard, jog shuttle, etc.: $169.40
Taig: $5,145
  • Taig 5019CNC: $2,995
  • Consew motor, pulleys and belt: $150
  • Frame upgrade: $500
  • TTS spindle & power drawbar: $1,500

Spindle Upgrade

The stock spindle motor on the Taig is a 1/4 hp motor, whereas the Tormach PCNC 770 has a 1 hp motor, and the 770M has a 1.5 hp. That's a pretty big difference. The Tormach also has spindle speed and on/off under software control. Whereas, on my Taig, I have to flip the switch for on/off control, and change pulleys to change speeds. The pulleys give me 6 different speeds, from 1,050 to 10,600 RPM.

After doing some research, I stumbled upon the Taig Lathe And Mill Owners Club on Facebook. This is a pretty active community, and finally got me onto using Facebook. There I learned about a very inexpensive motor upgrade using a sewing machine servo motor. The Consew CSM1000 motor is a 3/4 hp motor, so close enough to the PCNC 770. I purchase one from Amazon for about $100 and some pulleys and a new belt (another $50):
The first motor was defective, so I sent it back and got a replacement that works. For the price, the hassle was OK.

In order to use this new motor, I needed to mill a motor mount, order some pulleys and belt, and the bore out the larger pulley to fit the Consew motor shaft. I found a motor mount in the Facebook group that also had the CAM already set up (but you'll need to use less aggressive feeds with the stock motor):
Here are the two videos I created covering making the plate and boring out the larger pulley:

Frame Upgrade

Stuart Andrews has created a very nice upgrade to the stock from. For $500, you get a stronger frame, plus some much needed room in the Y and Z directions. You can find more information here:

I've received this frame and will provide updates here once I've rebuilt my machine with the new frame.

Sunday, November 4, 2018

Fusion 360 Cutter Compensation and Mach 3

Cutter compensation is a great way to dial in a hole to be a very precise size. I learned about cutter compensation from a John Saunders video How to Use Cutter Comp on a Tormach! WW180. In his video, he's using PathPilot on a Tormach. But I have Mach3 with a Taig, so the workflow is a little different. But not by much.

First, some background. Cutter compensation is done use a set of g codes: G41 and G42. Which one to use depends on the direction of cut. Fortunately, Fusion 360 handles choosing the correct one based on what you're trying to do.

Here's the high-level overview of how it works. Normally, Fusion 360 will calculate the correct location of the tool path based on the diameter of the cutter. In the picture below, you can see that it's moved the tool path for the cutter inward by half of the tool diameter.
In other words, Fusion 360 is handling the calculations to compensate for the diameter of the cutter.

Cutter compensation in Fusion 360, at least at the time I'm writing this, is only supported for 2D operations. 

Setup in Fusion 360

If you change the default In computer to In control, you're telling Fusion 360 that the controller (Mach3 in my case) will handle compensation instead. Here is how you make that change:

Once you regenerate the tool path, you'll see the following:

This may be a little hard to see, but now the tool path (the blue line) is exactly along the profile, rather than 1/2 a diameter away.

Setup in Mach3

Mach3 has a tool table. I have never used this before, which means I've always been using tool 1. To set a tool diameter in this table:
  • Click the Offsets tab
  • Click the Save Tool Offsets button
  • Edit the Diameter (D) cell for tool 1
  • Click Apply (very important, because it won't keep your changes otherwise)
  • Click OK

Edit G Code

You might think you're done, and ready to make small changes to the diameter (making it slightly smaller to make the hole larger). But that's not the case. Fusion 360's post processor for Mach3 emits g code that looks something like this:

G1 G41 X3.11 Y-1.65 P0.125
G3 X3.26 Y-1.5 I0. J0.15

Notice the P0.125 at the end of the line that contains G41. This tells Mach3 to use this tool radius instead of the value in the tool table, so you have to remove this. Additionally, I found comments that Mach3 doesn't like having G41 on the same line as other commands. So, I edited the g code so the above appears like this:

G1 X3.11 Y-1.65
G3 X3.26 Y-1.5 I0. J0.15

Once I made those changes, I was able to slowly change the diameter of the cutter in the Mach3 tool table until I had the hole just the right size. I started with 0.25 and then worked my way down to .244 (I made the hole in CAD slightly smaller than my target).