3 Attachment(s)
Having problems with aluminum engraving.
Hello everyone, long time lurker, but I am completely stumped and can't find information specific to my issues. I will try to give as much information as possible and a little backstory. Feel free to skip the first paragraph if you don't want the back story, but it might contain useful information. Note to mods: I'm sorry if this is in the wrong sub-forum.
I own a fabrication shop in California, and deal mostly with aluminum. I bought a cnc router (48"x48" working area) back a few months ago and have learned the ropes by making wood projects. The reason I bought it was for aluminum routing though. I'm currently using a liquid cooled spindle that appears to have a spindle RPM range from 1-24,000, I have been too worried to run the spindle under 6,000 rpm so far though. I have got to where I can make parts from aluminum with decent success, but engraving has been a real challenge for me.
I have .080(2.032mm) sheet aluminum I am trying to engrave for some information tags for my products. I started off with 5052 alloy but I don't think it machines very well. It seemed like it melted no matter what i tried with my feeds and speeds. I was able to get it to work, but it required too much sanding which was taking too much time. I then tried engraving some 6061 aluminum tubing (to test the other alloy) and it worked beautifully. I bought a sheet of .080 6062, but am now having issues again. I will attach pictures below.
I am currently using an Onsrud .020 SC SE 30 DEG engraving bit. The completed plate I made was made with a Onsrud .005 SC SE 30 DEG engraving bit. The tech at onsrud recommended a slow travel speed because of the size of the letters. The bits have a .0045 recommended chip load, but I have tried everything from .0038 - .005 with no success.
- The letters I am making are two different sizes. One is about 1/4" (6.35mm) tall, the other size is 1/8" (3.175mm) tall.
- I am trying to engrave in .080" (2.032mm) thick 6061 alloy aluminum at a depth of .010" (.254mm)
- I have been using 30 ipm for the travel speed because that was the maximum the tech recommended for travel speed.
- I have tried 8000, 7000, and 6000 RPM for the spindle speed. giving me chip loads of .0037 .0043 and .0050 all with about the same results.
- I do not have a mist attachment, but I hold an air hose on the work piece while it is routing. I have tried both dry cutting, and using soap. I did not get a mist attachment because I was worried that the spray would contaminate the aluminum making it difficult or not possible to weld.
Here are the issues I am having:
- I surfaced my spoil board, but the cut depths still vary. I am only trying to engrave 4 plates at a time. The stock size is 5.5" x 14" (14 x 36 cm). I am clamping the material to the spoil board with 2 clamps on each side and nothing on bottom and top. I do not have a vacuum table, so I am trying to keep the metal on the small size to minimize any up/down movement of the material while machining. I think the depth of cut issue is caused by not perfectly flat material, but I'm not positive. The engraving cuts look better when they are more shallow than when they go deeper, but if I go any more shallow on my depth, it won't engrave the low parts of the metal.
- I am not sure if the material is moving at all. It is moving any it is too slight to be able to tell. I have it clamped down very well on the 5.5" sides but don't really have a way to clamp it down on the 14" sides.
- I am not sure if the material is melting, or just not cutting chips all the way out. the bottom of the cut looks decent, but the top of the cuts is pretty rough and does not scrape off easily.
- The aluminum tubing of the same alloy as the sheet I am currently using engraved beautifully. My thoughts are it might be more rigid? It might just be that it is thicker? It might be more flat and i'm getting a more consistent depth of cut? It's only 1" tubing so there is almost no chance of up/down movement as opposed to the sheet I am using.
- Should I be using a different cooling method like mist or putting oil down?
-One more random question, I have been getting the bit close to the surface of the work, then measuring the distance between the bit and the work surface. I then use g commands to bring it down until it is .002 - .003 above the surface and zeroing the Z axis. Is there an easier way to deal with this when I need to be this precise with the depth of cut?
Please let me know if I left out any information. Thanks to anyone who took the time to read this. I attached 3 images. 2 of them are showing the roughness of the engraving I am trying to do currently with the 6061 alloy. The other imagine is a completed plate made from 5052. The finished plate looks good enough but I do not want to have to scrape the letters out, paint it, then sand the surface off if I can avoid all those extra steps, It takes far too much time and doesn't look as good as I would like it to.
Re: Having problems with aluminum engraving.
It sounds like you're not able to hold that thin sheet of aluminum down firmly enough to get a good cut. With an upcut bit, there's a tendency for the material to be pulled up a little from the table, and then dropped as the chip breaks. The fact that you're getting much better results on a piece of tube (which wouldn't have this issue) makes me think this is a large part of your problem. You could try rigging a vacuum pod for these parts, or use some carpet tape underneath to stick it down to the table (or a sub-plate that's easier to stick to). You might try using your mister as well, since aluminum usually cuts a lot better with some lubrication. Try a piece cut that way to see if you really can't clean the residue off well enough to weld it; I've never heard of this being a big issue. And usually, you want to spin a lot faster for engraving with small pointed tools; I don't know why they told you to slow your spindle down that much. For the smallest letters, I'd be tempted to run flat out at 24k RPM.
To zero the tool, get a pack of ZigZag cigarette papers, and hold one under the tool as you move down by thousandths, moving the paper a little. When it pins the paper, you should be .001" above the surface.
Re: Having problems with aluminum engraving.
Quote:
Originally Posted by
4iSteven
Hey arewby, thanks so much for the advice. I have been using shims to gauge how far away from the material the bit is. It works decently, but specifically what I'm asking about is, is there an easier method to get close? Currently I jog the machine down until it's as close as I feel safe being. I then measure it with the shims and use manual g codes to move down in thousandths after that. It's a hassle and I worry about accidentally jamming that tiny point into the material and breaking it.
[As long as it's descending .001" at a time and you're sure it hasn't touched yet (hence the moving zig-zag), it shouldn't break. It is a hassle, admittedly. There are automatic zeroing systems, but they tend to be less precise.]
I was considering getting some double sided tape, but was worried it might not stick to the spoil board very well. My main concern was that it might not be a consistent height all the way though the taping job. Working within thousandths is intimidating to me. Even though I surfaced the spoil board, I'm still getting inconsistent cut depths from one side of the stock to the other. Should I not worry about these issues too much?
[Unfortunately, you do have to worry about this. When engraving to a shallow depth, even a small difference in level between one corner of the workpiece and another will show up dramatically, since the lines get wider as the tool goes deeper. If you've zeroed on a high corner, the low spots might not get engraved at all. If you're sure your stock is perfectly even in thickness, you can mount an aluminum plate to the spoilboard and surface that. This will give you something you can mount your parts on that matches the XY plane of your machine, which the tape will stick to.]
I was finally able to make some good engravings and if anyone was wondering what I changed:
- I pushed the bit in as far as possible to minimize deflection.
- I resurfaced the board.
-I set the z axis up in the middle or the work piece instead of the bottom left corner.
When you say up the spindle speed, would That also mean I need to up the travel speed to keep my chip size the same? If I didn't speed up the travel speed wouldn't melting become an issue?
The quality of the engraving is acceptable now, but still not ideal. I have been considering ordering some double sided tape for a while now. Thanks again tor the response.
It's good if you're making some progress - keep trying things, one at a time, and gauging the effect. I doubt you'll actually melt the aluminum by spinning faster, but would suggest some lubrication to stop it from sticking to your tool. Try feeding slowly at first, but if all seems okay, then up the feed until you like the chips better. It's tricky to estimate chip-load on an engraving tool, since that varies depending on depth of cut. At the very tip of a pointed tool, there's hardly any cutting diameter, so the chips will be very small.
Re: Having problems with aluminum engraving.
Engraving is "black magic"
The harder the aluminum the better. I would not try to engrave 5052. Saying you have 6061 is not enough information. 6061T6 is hard enough to engrave, 6061T0 is too soft. 2024T3 is harder and easier to engrave.
I learned lots, the hard way. As "machinists" we think of cutting into the metal a certain depth. When engraving, all you need to do is scratch the surface a bit. The fine engraving bits can't take much depth or the point chips, I use a microscope to inspect the tips. I have decided that it's not the depth that brakes it but the force that depth exerts on the tip. I powdercoat panels and engrave through the powder coat, so I need to cut dry. I fought for many hours trying to get consistent depth over the area of the panel. I experimented with lots of systems including a vacuum table that I surfaced each time, no luck.
What finally worked will make educated machinists shudder.
I made a wood tray with sides 3/4" high. I place some very soft 3/4" "egg crate" foam, like from a cushion, in the tray. I lay the panel upside down and put strips of fiber packing tape on it extending out the ends and sides. Then flip the panel right side up and position it by pulling the tapes to the sides of the tray. Since the tapes are horizontal and the tray sides and foam are the same height it all stays level. The tape will not stretch and holds position very accurately. By experimenting I found if I set Z0 at the surface and "cut" .020" deep, I get great consistent results. The foam flexes and thereby limits the force exerted on the bit, but is even enough in compressive force that small variations in height don't affect it.
Re: Having problems with aluminum engraving.
Quote:
Originally Posted by
planebuilder
I made a wood tray with sides 3/4" high. I place some very soft 3/4" "egg crate" foam, like from a cushion, in the tray. I lay the panel upside down and put strips of fiber packing tape on it extending out the ends and sides. Then flip the panel right side up and position it by pulling the tapes to the sides of the tray. Since the tapes are horizontal and the tray sides and foam are the same height it all stays level. The tape will not stretch and holds position very accurately. By experimenting I found if I set Z0 at the surface and "cut" .020" deep, I get great consistent results. The foam flexes and thereby limits the force exerted on the bit, but is even enough in compressive force that small variations in height don't affect it.
I'm having trouble picturing your setup in my head. Could you post a picture for this old guy? Sounds like you have the problem solved.
Re: Having problems with aluminum engraving.
An item to remember is the smaller the tip of the cutter,
the velocity and chip clearance goes to zero and you just kinda push metal instead of cut.
I experienced this with a 2" ball end mill on a stainless steel wing contour bond jig.
Mushed the metal , under the tip of the ball .
We put it on the 5axis, tilted the cutter and cut chips with the side of the cutter not the tip.
Right on the 6061 t6 advice
Re: Having problems with aluminum engraving.
Jim, this may give you a better idea of how I do it. On this one I have fiber fill from a pillow under it. You will notice a sheet of aluminum under the panel, that evens out the load, otherwise the ends of the panel would depress more than the center. The tapes on the panel have sticky side up and extend out a few inches from the panel, then i added tape to those but sticky side down to stick to the perimeter frame. One unexpected advantage is that I can do some non flat parts, without the backer panel, small areas at a time. On some irregular surfaces, I have even varied up pressure by hand as it cut, with a 6" ruler as a lever.
2 Attachment(s)
Re: Having problems with aluminum engraving.
Re: Having problems with aluminum engraving.
Thank you planebuilder :) That is very cool. Going to try it next time I do some engraving.
One more question. What is TPDR, and ENCODER? Never seen those on an aircraft panel before, but it's been about 30 years since I was in the cockpit.
Re: Having problems with aluminum engraving.
TPDR transponder for radar
Encoder for mode c to give radar altitude reporting.
Re: Having problems with aluminum engraving.
Quote:
Originally Posted by
planebuilder
TPDR transponder for radar
Encoder for mode c to give radar altitude reporting.
Ahhh. OK, just hadn't seen those terms before. Always just called them ''transponder'' and ''mode C''
Thank you :)
Re: Having problems with aluminum engraving.
I have had some joy with a vacuum table to hold down flat - cover all the rest of the vac table to conserve vacuum!
Then, if the engraving has too much burr on top, I simply rerun the program and repeat the cut. For some reason this seems to do a good clean-up. Slower of course, but often worth the better finish.
Cheers
Roger
