What's new
What's new

.008" Slitting Saw-Student needs help!

When in the cut, observe the teeth- as others suggest if they are packing off with material it will increase cutting effort and tend to deflect the saw. I use flood coolant to wash the teeth out as the saw goes around- its at least as important as lubricating the cut itself.

With careful control of how the saw is cutting its possible to hold .001 sorts of dimensions even with thin saws, in aluminum or steel. Managing the stress on the saw is important- the thinner it is the easier to cause it to warp which can also make the kerf wander. Might be you're seeing that- its quite difficult to feel how the cut is working in a Bridgeport, possibly even moreso on a CNC. I use an old production mill with table lever feed and its excellent for feeling the cutter work.

The progressive cuts are the right approach- I would make them even less. For the 1st few cuts I limit depth to approx the blade thickness, even a bit less. Once depth of the kerf is more than the tooth height then then I'll go up to no more than a couple times the blade thickness, and can keep going up to the full cutter depth. For such deep cuts, a wandering kerf easily causes the cutter to shatter because the flex gets progressively more acute the deeper you go.

Even for the thin grooves that means a bunch of passes; rpm and feed is going to be constrained due to surface speed of the cutter and chip evacuation from the teeth.

I do find its possible to speed up the table feed given a smaller depth-of-cut, but the rpm and cutter surface speed is going to impose an upper limit. Aluminum is easier on tools than steel, so you might be able to push towards max feed and cutter rpm; but be ready to burn up the tool on the way to finding that limit.
 
Stick a wood wedge length wise down the completed channel before moving to the next channel. You want it fairly snug to support your next wall- not so much it folds the previous wall over.

No matter what you run saw (or any cutter) there is a side load from the chip in the shear zone. The bracing helps contain that load.
 
I'm kinda surprised so many answers posted remain with traditional machining...I would think (?) that this is a laser job or water jet or ? something more hi-tech.

I also imagine this sort of cutting, if done with traditional steel cutters, would be done not one slot at a time but in gang fashion with some sort of multi-blade comb-looking cutter. Sort of like a fin comb. I also envision this done with either tons of coolant flood and/or with the slots vertically oriented, not lying flat. Start at the top and cut downward.

Finally, I have to wonder why the research is being done on such a small scale. It seems it could be done scaled up, with something like .080" slots with a .100" land, then extrapolated accordingly. More human-sized. And if there's one thing engineers love...it's extrapolation.

I also wonder about the ability of fluid to run through a channel that is .008" wide. Yes, it will fit in a channel that small but getting to flow in a channel that small with any sort of regularity seems questionable. It better be very thin fluid without any surface tension, air, or sticky-ness.

What I don't like about the OP's method is it sounds like something I would do....knowing I was using a makeshift method due to my laziness and stupidity.
 
Last edited:
Remember it’s a university shop. Access to more sophi technology my or may not exist. There can also be a lot of emphasis on making do, either due to the Byzantine procurement process, or the individual professor holding the purse strings. Some grants also just don’t have much money.

Since they are starting with a BP hopefully it has a power feed in one axis. That will at least make keeping a uniform tooth load easier. I would finish each groove to depth and then fill it with some shim stock to prevent it from being folded over when doing the next one. Anything will do, if it’s slightly undersized a drop of CA glue will both restrain it and fill the remaining gap. When finished just drop in some acetone to get rid of it.
 
At some point I had to do something similarly unreasonable to this, but with round holes. I would cut the first slot, drop a same thickness shim in it for support, but the next slot, and so on.
You might be able to progressively fill each slot with something solid that dissolves or melts out later, but I’d start with the shim strip.
For my round holes I used class X gage pins 1 um under the hole size, but 3.5 um smaller worked too.
 
When in the cut, observe the teeth- as others suggest if they are packing off with material it will increase cutting effort and tend to deflect the saw. I use flood coolant to wash the teeth out as the saw goes around- its at least as important as lubricating the cut itself.

With careful control of how the saw is cutting its possible to hold .001 sorts of dimensions even with thin saws, in aluminum or steel. Managing the stress on the saw is important- the thinner it is the easier to cause it to warp which can also make the kerf wander. Might be you're seeing that- its quite difficult to feel how the cut is working in a Bridgeport, possibly even moreso on a CNC. I use an old production mill with table lever feed and its excellent for feeling the cutter work.

The progressive cuts are the right approach- I would make them even less. For the 1st few cuts I limit depth to approx the blade thickness, even a bit less. Once depth of the kerf is more than the tooth height then then I'll go up to no more than a couple times the blade thickness, and can keep going up to the full cutter depth. For such deep cuts, a wandering kerf easily causes the cutter to shatter because the flex gets progressively more acute the deeper you go.

Even for the thin grooves that means a bunch of passes; rpm and feed is going to be constrained due to surface speed of the cutter and chip evacuation from the teeth.

I do find its possible to speed up the table feed given a smaller depth-of-cut, but the rpm and cutter surface speed is going to impose an upper limit. Aluminum is easier on tools than steel, so you might be able to push towards max feed and cutter rpm; but be ready to burn up the tool on the way to finding that limit.
Thank you for the advice, I will try limiting depth per pass. I have a few of the HSS blades, so it is worth it for me to try to push towards the limit!
 
Stick a wood wedge length wise down the completed channel before moving to the next channel. You want it fairly snug to support your next wall- not so much it folds the previous wall over.

No matter what you run saw (or any cutter) there is a side load from the chip in the shear zone. The bracing helps contain that load.
Thanks for the suggestion! I'll give it a try.
 
I'm kinda surprised so many answers posted remain with traditional machining...I would think (?) that this is a laser job or water jet or ? something more hi-tech.

I also imagine this sort of cutting, if done with traditional steel cutters, would be done not one slot at a time but in gang fashion with some sort of multi-blade comb-looking cutter. Sort of like a fin comb. I also envision this done with either tons of coolant flood and/or with the slots vertically oriented, not lying flat. Start at the top and cut downward.

Finally, I have to wonder why the research is being done on such a small scale. It seems it could be done scaled up, with something like .080" slots with a .100" land, then extrapolated accordingly. More human-sized. And if there's one thing engineers love...it's extrapolation.

I also wonder about the ability of fluid to run through a channel that is .008" wide. Yes, it will fit in a channel that small but getting to flow in a channel that small with any sort of regularity seems questionable. It better be very thin fluid without any surface tension, air, or sticky-ness.

What I don't like about the OP's method is it sounds like something I would do....knowing I was using a makeshift method due to my laziness and stupidity.
Thank you for the suggestion about the fin comb/gang fashion. In my head it seems like having multiple blades would actually help support the ridges between them.

As far the validity of my method, it is certainly not due to laziness but is definitely stupidity. Like with all new endeavours I don't know enough to figure out what I don't know. That's why I'm turning to more experienced hands, thanks for your help!
 
Remember it’s a university shop. Access to more sophi technology my or may not exist. There can also be a lot of emphasis on making do, either due to the Byzantine procurement process, or the individual professor holding the purse strings. Some grants also just don’t have much money.

Since they are starting with a BP hopefully it has a power feed in one axis. That will at least make keeping a uniform tooth load easier. I would finish each groove to depth and then fill it with some shim stock to prevent it from being folded over when doing the next one. Anything will do, if it’s slightly undersized a drop of CA glue will both restrain it and fill the remaining gap. When finished just drop in some acetone to get rid of it.
Thank you for the tip on the glue!
 
Thank you for the tip on the glue!
Aluminum is best machined fast, it can be cut on a table saw, no problem. In your case the Bridgeport and slotting saw are fine. I think you just need better support for the saw. It should have washers maybe 1/8 or 3/16 thick on both sides and expose diametrically only the teeth. The washers should have the saw side relieved from the center out to near the edge to concentrate clamping near the teeth. You need a course tooth saw as mensioned. Also as mentioned 6061 T6 is important. Spray coolant for lubrication of the cut is CRITICAL in aluminum. A hand pump spray bottle is fine. 1500 rpm and 2-3 IPM should run fine. You can gang 2 or 3 maybe if you arbor supports it . I would washer all in the gang. Good luck with your project.
 
As others have suggested, the gang saw idea with spacers just small diameter enough to clear chips from the full depth should be a winner. Run it fast and small depth with lots of coolant or wd 40.
 
Any chance of sending 2 saw blades out for resharpening such that they take .010 and .020 off the radius or diameter?

Then gang 3 saws together such that you move the part one slot over for each slot. Would theoretically get the job done 3 times as fast.

Or cut 3 or 4 grooves at once with 3 or 4 blades of the same diameter.

Machinist wax would work to support the slots already cut, if you want to cut say 3 at once then move onto the next 3 or 4.
 
Are you cutting climb or conventional?

Can you slip supports into each slot after you cut it so it can't be squished by the next cut?
 
The swiss made carbide saws work much better if you can get a hold of one of those. Your tooth count, feed and depth of cut sound pretty reasonable. With a carbide saw at 2000 rpm or higher you should get a pretty good result.
 








 
Back
Top