CNC problems: Clamping (PLEASE HELP!)

Hey CD,

We’ve been cutting parts on our OMIO for a full season now and have come across a fairly troubling problem that we can’t seem to solve. Whenever we cut plate with our CNC, we get massive warping around the middle of the piece, which results in pieces losing tabs (and hitting our bits), not going through pieces on the edges of the plate, and putting way too much wear on our poor onsrud bits. We’ve broken 3 of the bits in 3 weeks. As you can see in the pictures, the piece seems to warp around 20-30 thou at worst (our tabs are 25 thou high).

Whenever we cut plate, we do our bearing pockets first (1/4" endmill), drilling operations (#10 and F split point), and finally our pockets and cutouts. We slot with 30 thou doc at 268 Hz (1 Hz = 60 rpm) and 33 ipm. We clamp our 1/8" plate over 3/4" MDF and clamp with 4 clamps. We know our feeds and speeds work fine because we’ve cut tube with similar f/s and it works fine.

With almost no time before our first competition, we’re doing anything and everything we can to try and fix this problem. If you have any questions, I’m glad to answer them; we just really need this problem fixed as fast as possible so we can get some last minute refinements made.

Here are the pictures: https://imgur.com/a/QkSt3

  1. Add some hold down holes in the areas between parts in the CAD or CAM software. Run this “hold down” program first, stop the machine, add hold down screws, then start the part program. Make sure your part program has enough retract to clear the hold down screw heads.

  2. Use double stick tape. Strategically placed is best because it can gum up your bit when you cut through the material into the tape.

  3. Vacuum table is super nice, but pricey.

Hold down screws work great (a small wood screw and washer). We’ve found that most of our parts already have conveniently placed #10 holes on the part that we can use.

This is what I do. Extra lazy version: drill all the holes first in one program, use them as your hold-down points, run your profiles program.

Remember - your cutter is an up-cut, it will lift the plate in the direction it is the most flexible. tie-down screws will help this tremendously.

I used to do something similar to #1. I’d lay the plate out on some 3/4" wood, clamp down in the corners, then drill all the bolt holes. I’d sink some short wood or sheetmetal screws thru the bolt holes and into the wood. this will prevent the metal from pulling up. definitely need to make sure the tool comes up high enough in the z direction to clear all the screw heads. you could still do tabs if you wanted…or cut full depth since the screws are holding the part down.

Apart from using hold down screws try using a single side of the cnc table since its a corner you can use 3 clamping point for the cnc and that really gives it a big boost and prevents that sort of stuff from happening. (believe me it happened to me to).

I see many holes begging for screws.
I do all holes first. Add screw even when running. Then pockets,cut out. I add screw on outer area to reduce chatter.

All of the this. Use DOZENS of screws! You fasten the part to within a thou of its life.

Agreed with the screw holes. They will save your part. Also, check the feeds and speeds, and what your manufacturers recommend. Often times tooling manufacturers will be your best friend when it comes to feeds and speeds. They want their tools to work well so you go back to them. They (usually) won’t lead you astray. I will often have hold down holes added to parts from the designers so that they aren’t placed wherever.

Also, don’t forget, you need to have a way to clear the chips so you aren’t recutting. This can increase tool wear and decrease your tool life.

I see you have a nozzle, is it a mister, or just compressed air? Make sure it is running either way, but a coolant mist definitely helps with bit life by keeping the part and bit cooler. If you are running a long run in aluminum, you may need to give the router a rest and let it cool down a bit in between parts.

The warping could also be due to the metal having a slight warp in it. But that warp is likely causing the bits to pinch and bind.

All else fails, you can take a smaller cut depth. It will take longer, and could increase your heat, but you will be less likely to have the bit break.

The one glaring thing that I see is how long your bit is. A lot of your breakage problems could stem from the bit just being too long, and trying to take too deep of a cut. I have snapped a lot of 1/8" bits in my day because they were too long and prone to snapping.

Thanks for all the responses guys, based on your comments I think I found out what our troubles have been. Just for some quick background and information, we have been using our manufacturer feeds and speeds with a constant air blast throughout the cuts and have tried 6-7 hold-down screws before much to the same effect I described earlier. Our problem was most probably the up-cut from our bearing operations before the drilling. By having the bearing operations then, we pre-warped the plate. We just did a new operation with the quick switch of putting the drilling before the bearing cutouts rather than after, and then putting some quick hold-down screws. With this fix we seem to be back in business! Again, thanks for the responses; this kinda stuff is what makes the FIRST community so awesome.

1 Like

From your first picture, it appears as you are using a boring bar to machine the slots. That is not what they are designed to be use for. End mills are ground with a spiral center to help lift the chips out of the cut area. You do have a heat problem as can be seen with the chips melting and fusing back together. Using air as a coolant is not near efficient as water and soluble oil for removing heat. Unfortunately most routers are not set up for liquid coolants. However speeds and feeds can be adjusted to help overcome the heat issue. Since you can’t use water, I would suggest using a 2 flute carbide end mill. The fine grain of the carbide has less chance of the chips clogging up during machining. They actually make reverse spiral ground end mills that push the part down instead of pulling up as the cut is made. But at an extra cost…

http://www.wcproducts.net/catalog/product/view/id/939/s/wcp-0053/

that’s an end mill

Please don’t use a down cut tool in aluminum. Aluminum recut is a nightmare and down cutters recut like crazy.

Holes and screws all the way. Tape and vacuum are typically insufficient for metal, but perfectly fine for plastic and wood (and pink foam!)

An Onsrud 63-620 can happily cut 1/8" aluminum in a single pass at 16000 RPM and 10 IPM. It is astoundingly unhappy at the same speed and feed cutting only half-way through (i.e., 2 passes).

Try going full-depth and see what happens. 832 does this with only manual air blasts on occasion for chip control, and the bit is not even slightly warm at the end of the cut.

A mill is not as effective at high speed as a router bit. Our spindle only goes down to 3000 RPM, and so we don’t use mills.

FWIW, the recommended chipload for a 63-620 is 0.003"-0.006". Running at a higher IPM (closer to 50ipm) and a lower DOC might net better results and extend tool life. 299 used to run endmills very slowly, but they doubled the feedrate and it cuts much better now.

for end mills, I would recommend the LakeShore carbide aluminum end mills for 1/8 inch 2 flute not 3.

http://www.lakeshorecarbide.com/18variable2fluteendmillforaluminumzrn.aspx

This season we had to machine lots of plastic intake arms because they are on the leading face of the robot outside the frame perimeter and drilling the holes and screwing the piece down worked great, it also allows you to not of to use tabs.

Also as a substitute for double-sided tape, you could go with painters tape and superglue.

I know it was the aluminum that was bowed but machining the plywood waste board down so that it is flat with the machine could help out with the flatness of your part.

I also noticed that your clamps are only in the corners placing clamps in the middle of the part does also prevent bowing.

  • Kyle Warren team 2052 C.N.C. expert

I agree with the others about using cutters designed for Aluminum on routers. Our team got a couple of Onsrud 1/4 inch bits before off-season last year. Only one of them has been taken out of the package and it is quite literally the only bit we have used on Aluminum since. It has worn, primarily in the tip which starts as basically a point, but it still cuts great. Be sure to use some kind of coolant though. Cold air blast works well for us.

One janky way to reduce that warping as well as vibration is to simply push down on the stock with your bare hands. If that is a little too sketchy for you, use a piece of wood. It helps out in a pinch for those times when you think to yourself “I should have put the tab THERE, whoops”.

What IPM, RPM, and DOC do you run with that 2-flute? Seems like you’d need to go pretty fast to make it work.

you would have to do some experimenting with your machine but i use the nyc cnc speeds and feeds calculator and Lake Shore carbide gives the recommended information for their end mills

https://www.nyccnc.com/getting-started-feeds-speeds/

We use a lakeshore carbide 2-flute 1/4’’ endmill for bearing pockets and other adaptive stuff, and an onsrud for slotting. Aside from the work holding problem mentioned in this thread, we haven’t really had any issues at all.