I’m curious how everybody who uses a CNC router holds down their larger sheets. We have a 24x36 on our table but the MDF spoilboard has been warping due to wd-40 spraydowns and the metal itself warps as it cuts. On lower-end machines, it causes an increases chipload and therefore lost steps. I’ve planed this table down several times and am considering getting into vacuum hold downs, but I hear they don’t play well with coolant. What do you use?
If you have any holes to run on your parts you can run a drill program fist and use those to screw/bolt down where individual parts will be. We’ve had good luck with this, but we don’t have a sacrificial board, ours is all slots for clamp mounting.
Anywhere you’re possibly drilling holes, or could sacrifice to make them for accuracy’s sake, go ahead and make a fixture plate that you can mount your finished part on top of. Just take a piece of stock the same size/larger and tap those holes, screw part to fixture plate. Other option would to make a fixture plate that you could mount some work-holdings onto…
Lots of clamps around the edges and thin double sided tape seem to work well. I recommend getting plastic clamps (like Irwin Quick-Grips) so collisions between your cutter and your clamp aren’t as destructive.
A fixture plate is nice, but hard to do when your stock is several feet in length.
Here is what I’m doing lately.
Aluminum sheet stock, I’m leaving on the sheathing layer of plastic. I then spray headliner adhesive (for attaching a fabric headliner to a car) on both the plastic backing and to a sheet of clean 3/4" plywood. Let them air dry for a minute, then press the pieces together. I am getting really clean cuts using his method.
On our CNC mill when we want to run sheet parts, we install a 32" x 16" tape plate (~1.5" thick block of aluminum with a 2" x 3" spine on the back) clamped into our 3 vises. We then use 3M Flexomount 412DL 2-sided, foam core tape to hold the sheet to the plate. This tape is .020" thick and we buy it in 1" wide rolls. We fluctuate how many strips of tape we use depending on how big the parts are we are going to cut. This tape is geared to the printing market so it holds up well under our flood coolant.
We set up our programs to just punch through the sheet material by about .008" so we don’t cut the tape plate itself. This tape is a little pricey and sometimes difficult to find in less than 32 roll quantities but if anyone is interested in trying this out, PM me and we can possibly break down our large orders and sell smaller quantities.
Happy cutting!!!
We on 1678(and me personally at work) use the above methods as well as leaving behind tabs on some of the more troublesome parts.
I have a few things to say about sacrifice boards.
1678 is using a fine particle board as our sacrifice, it takes half a 4x8 to cover the table of our VeloxCNC and the full sheet only costs about $35. We use small sheet and wood screws straight into the sacrifice, in holes where possible, holding down edges otherwise(takes 4-8 screws to do it this way). We also have several blocks of plastic to the side of our sacrifice that have been machined in place that we use to clamp extruded square/rectangular tubing to to drill and machine(PM me if you want pics). When we plane down the board another couple times or so and machine into it enough to risk hitting the bolt heads holding it down we will take it off, throw it away, then bolt a fresh piece down. We have gotten our mister working with WD-40 at a VERY FINE rate that keeps the sacrifice in relatively good shape even after heavy use. If you see droplets you are using WAY too much lube. You cannot use a water based lube(even with a fine mist) with the stuff because it swells and warps, requiring much more frequent resurfacing of the sacrifice.
Greenbotics where I work uses a 1" thick PVC foam sheet(now about 0.85") that is bolted to the table, it is far more expensive up front but has many benefits. The biggest upside is being able to use any lube that you want as it won’t adversely affect the sacrifice, the water based stuff is much cheaper. The PVC foam is also much more dimensionally stable in areas that have changing humidity levels or many other environmental factors. That means that you can machine parts that require a reasonable amount of depth accuracy such as ±0.005". Another big upside is that once you have planed the sheet down enough you can just glue on another sheet on top of the original and have WAY more material to plane off than the first go.
We’ve been doing similar. Our first op for any new part is to cut a set of screw holes around the part. The second op is to then cut the part, leaving it tabbed into the sheet. The beauty of the screw hole job is that it tells us if we have Z set right to cut all the way through the sheet over the area that our parts are being cut. If the screw holes don’t go through, the pockets won’t either.
We’ve been using a waterproof MDF which does not swell. I’d say it is within 0.040 of flat on our machine. We are always looking out for better materials. Do you have a part number/source for the PVC you use at work? Price of aluminum >>> price of endmills > price of MDF, so we should be able to afford a slightly pricier MDF to make life easy.
That much variance would drive me NUTS! I get unhappy with even 0.010 out of flat.
We buy our PVC foam sheet from Professional Plastics http://www.professionalplastics.com/PVCEXPANDEDSHEET
I would suggest liberal amounts of PVC cement or contact cement to bond new layers.
It’s pricey but Misumi sells 250 mm T-slot that can be mounted on a extrusion frame. This allows t nut clamps to be moved all around. I used a good dense MDF board leveled. I drill 4 holes in the corner of the AL plate. The Al plate is screwed down onto a good flat piece of 1/2" plywood into the MDF. Has worked very well so far but is not Ideal. Had problems with double sided tape building up and gooing the mill. Also interfered with chip ejection on the last cut thew pass. We have an X-carve stock, no stiffing mods. When the part allows , we use a 1/4" 2 flute 45 degree helix ticn coated end mill designed for AL. We get clean cuts on 6061 at 15 IPM and .01 DOC. Can go faster but cuts are not as clean. For small precise cuts have been using a 3 flute 45 helix .125 end mill at 10 IPM and .003 DOC. This may seem slow compared to those with real router tables but, we only have 700$ in this. It’s been cutting all week. With some mods the capability can be increased. It’s been a learning experience. We have had some friction stir welding experiences in the beginning. For next year with some mods it will be better. Software also is important. Next year we intend to master HMS Express to give better tool path planning.
Last night we cut some 7075 AL and my what a difference. It cuts so much better than the gooey 6061.
So far the X-Carve while not pro grade has been of great value to our build season.
Magnetic tables work well, but are pricey. With sheet you can use ferrous material (scrap) to hold down your non-ferrous. May not be viable for your team, but you asked for options.
for holding down the edges you can use Cleco clamps
They come in some Cleco sets and you can open and close them with Cleco Pliers They’re nice and small so you can get them into places where there’s really low clearance.