Plate Workholding for CNC Mills

Hello all. Recently our team has gained exclusive access to a 2003 Gain G16 Knee-Type Milling Machine that was converted to a CNC Machine with a CENTROID M-15 Control Box after our school’s IT department decided they were never going to use it. This machine has sat unused for the last ~10 years, so I have spent the last 2 weeks restoring it, configuring and tuning the feedback system, tuning the DRO outputs, and overall learning how to use the machine. I have gotten to a point where it correctly interprets GCode exported from Autodesk HSM, and the DRO outputs are now accurate to 1/4 thou.

The biggest question we are having right now is work holding. We intend to use the machine primarily for cutting out gearbox plates and support brackets, most of which will be made out of 1/4" or 1/8" aluminum plate/sheet. We also intend to do some cutting with 1x2x1/8" box tube. Does anybody have any experience with a jig system that allows place-and-go cutting of box-and-plate? I’ve attached a picture of the mill from the day we got it (it is now much cleaner, I promise :slight_smile:)


Tube is easy I would recommend a double vise setup. Plate on the other hand is much harder, we used to use a set of custom soft jaws with parallels machined into them and it worked ok but we had some bowing issues with wider plates, this year we switched to making fixture plates for most of our gearboxes this has worked the best in my opinion.

1 Like

How did you machine the fixture plates? Do you have any pictures of them?

We put the fixture plate in some vises and just ran the same drilling operation as for the plates, tapped the holes and bolted the plate stock on top of it.

Edit: the reason those fixture plates where so large was because we where running 4 or more plates on each fixture.


What is the manufacturer of that tapping fixture?

I believe it is this one

So a little bit different: The Crude (but Effective) Way and the Machinist’s Way.

Crude has a 3/4" MDF table fastened to the machine’s table using T-bolts. We then use the CNC to drill a series of (strategically-placed) 1/8" holes in the plate-to-be-machined, holding it down with a couple of binder-head screws (not a lot of side-to-side forces when just drilling). Then we use screws through the 1/8" holes to hold everything down to the MDF and cut out whatever it is. Plan on replacing the MDF ‘spoiler board’ every week or two.

Machinist uses the stepped clamping system to hold things down, with a set like these. There still needs to be a spoiler board beneath. Downside is setup time and possible inadequate hold-down in the middle areas. Then there is the issue of managing the workpiece after is is completely cut out. Better for things that are not plates though.

Since you can put in the holes as needed in the CNC design phase, the screws can be very effective and not interfere with your cutting tool.

If you are going to use a certain material often - say, 1 x 2 rectangular tube - have the machine build a holding fixture for you out of glued-up MDF, or for the same size plate (say, 12 x 24) create a shallow pocket in the MDF to hold the material laterally. See Tube magic

1 Like

These are a little pricey but I love them.

These mini-vises

With a SMW fixture plate that will fit your machine like THIS

These fixture plates once true-ed into your machine make subsequent work holding really easy. The mini-vices give you almost complete access to machine the part and 1 inch of clearance to the fixture plate.

I also use a cheap 3 jaw lathe chuck that can be attached to the fixture plate with these for holding round stock to mill.

If you do use MDF I don’t recommend using flood coolant as it would probably warp the MDF causing your part to not be parallel to the table.

The solution i’ve seen that I like is to use a sacrificial “riser” that you can attach the plate to. A bunch of other things I’ve seen are just using milling clamps to hold it to the table or even vacuum workholding from Pierson Workholding

Actual lumber is a bit better than MDF. 548 makes our wasteboard out of 2x12’s. They need to be resurfaced every now and then by just milling them down a bit with a large cutter, but that is mostly due to part cuts going too deep. It doesn’t swell that much, and definitely doesn’t lose strength. We use a mist system but we are often… Aggressive with our liquid quantities, so the wood certainly experiences the moisture.

Why not just use a vice? 254 does it. As long you don’t go too big with your gearboxes it’s not a problem. Once you get into large territory you can make a fixture - but this is one of those things you probably only need to do once a season. 2x1 tubes also fit inside a vice.

4414 made a pair of these.

We only use the outside 2 vices. All the holes are tapped for 1/4-20 bolts. Every single tube on our robot is rough cut to +.25 on the cold saw then milled to length. Because of this all the tubes need to hang over the right side of the jaws a few inches but the endless amount of x stops makes this painless.

We have run plates in it before but we tend to our smaller mill for this using the method linked by mike above ^. We have gotten away with milling some massive plates (around 8 inches in the y, i would have to check the exact number) by facing and milling an edge into a pair of soft-jaws that lets us get a few more inches out of the vice opening.

1 Like

If it’s too big to fit in a vise, we typically flip the jaws on the vise so that they are on the outside, clamp a 3/4-1.5" thick plate in them (usually spanning two vises) of whatever depth maximizes your Y axis travel and then pick strategic holes that exist in the part you want to cut and drill those clearance holes into the part stock (by clamping the part stock down to the tool plate (we use kant-twist clamps, but you could use toe clamps, c-clamps, whatever) and running your program.

We then shift our work coordinate system so that we aren’t drilling into the same spot we just drilled the clearance holes into and drill/tap matching holes into the toolplate. Then we bolt the sheet down to the toolplate through the holes we drilled and contour the part.

This generally yields higher quality results than our preferred method of clamping the raw plate stock into a vise, but it is WAYYYY slower and you often can’t chamfer all your contoured edges (due to the tool getting too close to the bolt heads holding down the part), which is a very 1st world problem for us. This method is unavoidable if the part is thinner than 1/4" and bigger than 4" or so, though.

It works a lot better on the router where you skip the drilling and tapping of the toolplate and just shoot wood screws in to hold the part down - saves a lot of time compared to doing it the more legit way on the mill.

We typically mill in 2 setups:

  1. Plate stock clamped in vice and all holes drilled and general boring operations.
  2. Then the plate is bolted down to a jig (which is clamped in vice) .
    The black post represent the hold down bolts.
    The jig fixture is drill and tapped for 5mm bolts on a 1" pattern w/ 1/2" offset on subsequent rows.

We utilize tabs to hold the stock / plate together when milling.

low key very jealous of that SMX. My old team had a crappy precision matthew’s mill. The x axis vibrated 8-9 thou when you cut along the y axis, even with the x axis locked.

We like the machine itself, it’s very rigid and accurate but the controller is very hit or miss. It basically just runs windows xp with some proprietary software that has lots of bugs.

Interesting. I use traks at college all the time now and the only error I ever get is when I accidentally set my tool offset on the right side… Do you upload a .cam or .mx2 file from mastercam or do you write the cycle on the interface itself? I’ve also heard that the 2-axis controls are less finicky than the 3 axis with z axis control. Maybe that’s the issue and it’s not user or operating system error?

Not to derail too much, but we have the EMX which seems to be software limited to a given number of lines of code. Is this true on the SMX? If not have you checked the amount of memory it has (just so I can double check it is a software limit on our control). I’ve also always been curious is we could just chuck some other piece of winxp (NT?) cnc control software on it to circumvent these issues but I don’t really know of any cnc software that level of support for old hardware.

We upload it as a .nc file. And we have noticed that the z axis is the most fussy.