[ironspider]

Greetings all,

I have built a CNCRouterParts 4896 with a 1.5kW air spindle (NEMA 34). I have to cut some pieces (just profile, nothing intricate) from 1/16" (.060) 304 stainless steel. The pieces are basically rectangles with some holes profiled in them and are about 4"x1.5" (I'll attach a pic below).

For awhile, I had been convinced that I couldn't cut this on my CNC (and was getting ready to pay a guy with a laser to cut it) but, after playing around with the CNCCookbook feeds and speeds calculator I think I came up with a "firing solution" that doesn't generate any errors (and has RPM above the 8000 minimum that I see a lot of posts reference?). So, I'd like to get two pieces of info from the community, 1). Does this setup look like it should work:

Proposed settings for .060" Stainless 304 cutting (#2B Unpolished Mill):
Tool: 1/8" TiAIN Carbide Endmill, 2 flutes
Stickout: .75
Cut Depth: .02 per pass
Cut Width: .125
RPM: 8710
Feedrate: 12.54 IPM
Plunge: 6.2

and 2). I don't have any cooling solution. Do I need one for a cut like this? Does anyone have a "Cooling for dummies" type link to what I might need to add to my setup (are there ebay kits? start kits from another source? Do I just spray water on it from a spray bottle when I see smoke? Do I shoot it with WD40? If so, how often?)

Thanks for any tips/advice you can give me!

[Spk64]

The issue you may have is any pauses in the cutting and the material will work harden. This will make it much tougher to cut even with carbide.
Need lots of coolant as at those speeds your part and tool will heat up very quickly.


Sent from my iPad using Tapatalk HD

[wizard]

Greetings all,

I have built a CNCRouterParts 4896 with a 1.5kW air spindle (NEMA 34). I have to cut some pieces (just profile, nothing intricate) from 1/16" (.060) 304 stainless steel. The pieces are basically rectangles with some holes profiled in them and are about 4"x1.5" (I'll attach a pic below).

Does it really have to be 304. Generally you don't use 304 unless it will become part of a weldment.

For awhile, I had been convinced that I couldn't cut this on my CNC (and was getting ready to pay a guy with a laser to cut it) but, after playing around with the CNCCookbook feeds and speeds calculator I think I came up with a "firing solution" that doesn't generate any errors (and has RPM above the 8000 minimum that I see a lot of posts reference?). So, I'd like to get two pieces of info from the community, 1). Does this setup look like it should work:

Pardon me here but unless you are using a very small tool 8000 RPM just sounds like a lot.

Proposed settings for .060" Stainless 304 cutting (#2B Unpolished Mill):
Tool: 1/8" TiAIN Carbide Endmill, 2 flutes
Stickout: .75
Cut Depth: .02 per pass
Cut Width: .125
RPM: 8710
Feedrate: 12.54 IPM
Plunge: 6.2

You can certainly try that.

and 2). I don't have any cooling solution. Do I need one for a cut like this?

Cooling? Maybe not so much cooling as a something to get the chips out of the cut area. If you have really strong flow on coolant that might do it but you might try blasting the chips out or even vacuuming them out.

Here is the nasty thing with stainless, those chips will be extremely hard and if the cutter try's to recut them it will either chip, crack or break. In fact the recut issue is so bad I'd look for ways to cut the parts in one or two passes, unless you can positively remove the chips.

Does anyone have a "Cooling for dummies" type link to what I might need to add to my setup (are there ebay kits? start kits from another source?

To start you need a tank and a pump. The problem is for stainless you want more that just flood coolant, you want enough pressure in the stream to flush the chips out of the cutters path. If you find the right combination of speeds and feeds you might get buy without coolant. However you need to blow or suck those chips out of the cut channel.

Do I just spray water on it from a spray bottle when I see smoke?

If you turn a carbide tool red hot it is a little late. Besides that never use plain water on a machine tool, it just leads to rust.

Do I shoot it with WD40?

WD40 only really seems to work well with aluminum. It is a marriage made in heaven.

If so, how often?)

The only real way to do coolant is continuously.

Thanks for any tips/advice you can give me!

You can try the speeds recommended but you need to acknowledges a few things. One is that Stainless work hardens real fast, your motion must be continuous. This means not stopping to look at you work just because. If the cut does work harden figure on the end mill being destroyed in seconds (actually it can be all over in less than a second). Wear safety glasses (this shouldn't have to be mentioned). Buy lots of spare end mills!!!!������������. Start with a feed rate reduced slightly from the recommendations. However with stainless you can't reduce the feed rate to much as you need to cut below the hardened surface. Generally you can hear when a larger end mill recurs chips, I haven't done a lot with a smaller end mill but I suspect it won't be pretty.

Finally is the piece does work harden in the slot I've had some success reversing direction. That is instead of trying to recut what has worke hardened and likely just broke your cutter get to the other side of the hardened area and revers direction cutting from what is the back side of the hard area. I've been able to save a few pieces this way, it is still hard on the end mill but then you need to figure the value of the part.

Give us a bit of feed back on how this works out for you.

[ironspider]

Wizard, thanks for all the tips. Is there another type of stainless/metal that might work well and not be too crazy-expensive? What I'm machining these two parts for are for a custom pinball machine I'm working on. At the bottom of the playfield you have guides that return the ball to the flippers, these are the pieces I'm cutting. On real machines they are .060" and I assume stainless--they seem very similar to the 304 test piece I got from McMaster. BUT, as you can probably tell from my complete novice-ness about cutting this stuff, I'm not exactly sure *what* type of stainless it is!

So, I'm totally open to using another metal, the only thing I really need from it characteristic-wise is to look good (the part will be seen for sure) and be that thickness, and not rust, and be able to take light hits from a pinball without denting or deforming.

If you've got another suggesstion for something that might not be as difficult but still meet my requirements I'd absolutely try that!

[Spk64]

I think any of the stainless grades would work in your application. The tough part is machining on a router.
Here is a chart showing the machineability of many materials to compare.
Machinability Comparison Chart - provides percentage scale of machinability of various metals indexed on 1212 carbon steel: carbon steels, alloy steels, stainless steels and super alloys, tool steels, gray cast iron, nodular cast iron, alumunum alloy

[ironspider]

Spk, so does that chart indicate which metals are "easier" to work with when machining? So, for example, a metal with a higher machinability number (like stainless 416) is easier to "machine" than the a metal with a lower number (like 304 stainless)?

[Spk64]

The higher the percentage the easier to machine. 416 will not have the corrosion resistance of a 303.

[ironspider]

I wonder if I could just use aluminum? Maybe like a 2024 Aluminum?

[msimpson99]

If you can do it in aluminum, it will be much easer to do than stainless. I think you will be going through bits like crazy on that machine milling stainless. With a good clamping system and some Oflute bits it would be very simple.

This is my machine (much like the machine you are using) cutting aluminum.


Here is my page on some auluminum booms I was working on. It lists the lubricant and bit I was using:
Cutting Aluminum Booms

I will add, the rigidity of your machine will dictate how well it can cut aluminum.

Also your ability to remove the chips from the cut path. Doing multiple passes on a very thin kerf can be problematic if you cant get those chips out of the kerf.

[wizard]

Wizard, thanks for all the tips. Is there another type of stainless/metal that might work well and not be too crazy-expensive?

Try 303. Stainless in any form isn't machining friendly. 304 though is alloyed for welded applications and doesn't yield good results.

What I'm machining these two parts for are for a custom pinball machine I'm working on. At the bottom of the playfield you have guides that return the ball to the flippers, these are the pieces I'm cutting. On real machines they are .060" and I assume stainless--they seem very similar to the 304 test piece I got from McMaster. BUT, as you can probably tell from my complete novice-ness about cutting this stuff, I'm not exactly sure *what* type of stainless it is!

There are many grades of what would be called stainless. Generally we use 303 at work for general parts.

So, I'm totally open to using another metal,

Hey if it is worth making it is worth making out of stainless.

the only thing I really need from it characteristic-wise is to look good (the part will be seen for sure) and be that thickness, and not rust, and be able to take light hits from a pinball without denting or deforming.

I would suspect Aluminum would dent over time. Even stainless might dent if it isn't hardened.

If you've got another suggesstion for something that might not be as difficult but still meet my requirements I'd absolutely try that!

The problem with a router is the minimal spindle speed you likely have. One option might be to saw the perimeter and then try to machine the what is left to final dimensions. This might allow you to run a slightly large end mill with a good feed rate. You could also try cleaning up the edge with a carbide burr. In either case you will likely have more spindle speed than you really want. This has me wondering just how low can you go with spindle speed and maintain good power?

If you only need two and the router can not handle it, you could use a German milling machine. That is a bench vise and a good file.

You might even want to try something like the above where the part is sawn almost to shape and the the edges cleaned up, but instead of an end mill try to grind the perimeter. It may or may not work as I've never tried to do something like this. However grinding wheels can be run at high speed (within the limits of whatever wheel you are using). The problem is this would require coolant and take for ever as you would only be able to step over a very fine amount. You might have to make a couple of hundred passes around the outside. I'm just thinking out loud here as to how to work with in the machinery you have. This might be a way to use the spindle at normal speed range where it likely develops rated power.

Another approach is to again rough cut to final dimensions and then use a belt sander to clean up the edges. With the right amount of effort this can be done to look good.

Find somebody near by with a real mill. Even big shops have to farm stuff out when they don't have the right tool. This gets to be expensive unless you find a local hobbiest.

Use your router to cut out a pattern and then ram up a sand mold and cast your part in the metal of your choice. Heretic you say. Well it is an option and you wanted options. But in the long run casting metal parts opens up a whole world of options when it comes to building your pin ball machines. Unfortunately it is also an art that takes a bit of time to master.

Another approach would be to make a carbon fiber / glass fiber laminate. Your router should be able to route this just fine. You might even be able to find the right laminate in stock someplace. In some some ways working with glass/carbon structures is a lot like casting metal in that you can realize shapes that would be hard to machine out of a block of steel. The biggest problem here is the need for proper cutters in the router as general purpose end mills don't work well in laminates.

Do the above with a really hard wood. The problem here would be resawing thin enough pieces to get a proper laminate.

Buy your stainless as thin flat stock that you bend around a form. Form your perimeter and then infill it with something.

Similar to above buy round bar stock and form as required. Both of these avenues will be easier with a welder and maybe a torch. Wire bending tools are easy to come buy or even make though. The thing here is that wire is used on a lot of commercial pin ball machines so this isn't out of the ordinary. You will also be need some flat stock to weld in for the mounting holes. Hand forming wire does take some time to master.


-–––———–––-

Well those are a few idea off the top of my head. As the old saying goes there is more than one way to skin a cat.