any tips before I build my grid plate

This is what I put together as my 36"x12" grid plate for my small VMC. I'm on a tight budget, and just getting started in CNC. I figured this would be a good project to run the machine on, and help me out with set up time later down the road. The through holes will be 1/2" for the locator dowels, and the blind holes are 1/2x13 thread. Any input would be appreciated, as I'd rather change the design now as opposed to later. The plate will be made from 1" mild steel.
https://www.cnczone.com/forums/attac...d=408296&stc=1

I forgot to mention, the through holes won't be drilled completely through on the finished plate. I was intending to only drill them .750 deep.

How is it to be located / fixed to the table ?

.... suggest either keyed or use a dowel thru the plate into tee slot ..... this is to keep the grid holes aligned to an axis for easier mount/unmount

.... you will find that you will want extra threads instead of dowels...suggest that you redesign each hole so that each hole can be later have a .20" deep dowel machined in, it doesn't need to have really have the dowels. So don't put something big in where you wanted something smaller.

Also manufacture/buy grubscrews to go into the holes to assist cleaning & to protect threads from swarf.

Blind holes could be a mess to clean from chips. Also, it could be a good idea to make all holes universal - so they could fit either a screw or a dowel. Or maybe use screw-in dowel pins?

https://i.ebayimg.com/images/g/z-IAA...a98/s-l300.jpg

Some good ideas there. My plate is only 1" thick. If I made all holes threaded to about .750, for the 1/2-13 thread, and cut the top .125 to 1/2" diameter reamed for good dowel fit that would leave me .625 for thread engagement. I could drill and tap a little deeper, but being it will be mounted in place when I do all the drilling and tapping I dont want to drill through and hit the table. So I'm thinking that will be enough thread engagement as long as I'm careful in my selection of hold down bolts, and try to use studs when possible.
I've been thinking on how I want to locate it on the table. I have considered drilling two opposing corner dowel holes through in to the table, and then placing dowels to keep it aligned to the table. It will be held down with t-nuts and bolts recessed in the plate.

Quote:

---

Originally Posted by ACC216

I've been thinking on how I want to locate it on the table. I have considered drilling two opposing corner dowel holes through in to the table, and then placing dowels to keep it aligned to the table. It will be held down with t-nuts and bolts recessed in the plate.

---

nah. do the dowels in-line... & try not to put holes into the table. You will regret doing it, especially when you want to machine without the grid. Try maybe keys in the tee slots.

Our grid is 32 plate...M12 thru holes @ 50mm pitch (every 2nd row offset 25mm) with cover screws to keep swarf from /assist cleaning the holes. Most jigs are just clamped to the table with clocking edge for aligning.
... Each jig has a datum hole to set work origin, so this eliminates dowels in the grid plate, so it also can be used on other machines.

Go all the way through. I assume that you're diagram is showing white for the threaded holes? Because out on the edge is where you want those guys for maximum clamping opportunities - you always want that one last damned threaded hole :)

I asked an old school machinist at work make up a plate to replace my cheap router bed as a background giggle when he had nothing else to do. Smaller rig, lighter loads, so 6mm dowels and M8 threaded holes, 32mm pitch and 1/2" plate. I mentioned blind holes to stop the dowels falling through and to stop crap getting onto the Y ballscrew but he set me straight - blind holes are the devil's playground. Swarf that jams in against the thread and won't come out, coolant that pools and turns to mud, rust potential on steel etc etc. Plus you lose that little bit more flexibility on the length of your bolts to fit particular clamps etc.

Instead we did all the holes right through, both dowel and threaded. To protect the mill bed during drilling, we just clamped it down onto parallels every 150mm or so. Then flipped the plate and I was handed a hammer and ball headed punch which I used to peen the bottom of the dowel holes, just enough that they wouldn't let the dowels drop through. Works like a dream, over a year on and I still love it compared to the old t-track deck.

So I'm just starting to get into this myself and have been trying to decide how I want to make a fixture plate. My question is this. Let's say I make one with straight through holes as you say and it's beautiful. Now I want to machine someone on this fixture plate. How do I protect it so I'm not drilling into it or cutting into it as I mill my pieces? Am I just putting a piece of shim stock 0.060" or something under it so I can machine through my part cleanly yet not damage my new fixture plate? I've been trying to figure out how this works. Then if I have 20 of the same part to make (for instance) do I need a new shim after each part or can I leave the old one in there even though it'll have tracks on it after the first operation? -Just looking for information on what you experienced machinists do because I'm new to this and trying desperately to learn.

I plan my toolpaths to keep them a good 2mm off the deck minimum - including allowances for tip to shoulder on drill bits etc.

If I have to drill or mill through, I mount the piece on parallels above the deck. Or in a vice. Worst case, I bolt it down through or around a spoil board. If you've got repetitive work for it to do, making a fixture plate with pockets under drill holes and full depth profiles might work for you.

So in general it sounds like you never drill through your material. If you're making a widget you leave a few thousands of material at the bottom so you never even have to go through into a sacrificial plate? But if this is the case, doesn't that make cleanup long and tedious? -I'm not criticizing I'm just trying to learn what's best. Not punching through parts has advantages, so I'm happy to learn about those benefits if it's the way most people do it.

I drill through all the time. And I do full height profile cuts. Drilling I mount a spoil board between the workpiece and the tool plate / bed and go to it. Or, if a little precision is called for, I clamp the workpiece on parallels which support the material either side of the holes but not under them, hold the workpiece say 5mm off the deck and go. Profile cuts, either a quick and dirty spoil board or I'll use dowels to locate the workpiece, profile to within 2mm of the bed, flip it and finish that 2mm in a separate operation.

I don't like using spoilboards as a rule - timber or plastic spoilboard under a metal cut feels sloppy and wrong. But sometimes they have their place.

please subscribe to my youtube channel.. i just posted on my G-code CNC PCB milling https://youtu.be/CNIyHB7awX4