[muibubbles]

So I've search High and Low, tried a WIDE range of settings and still cant dial it in.. I'm going broke from buying bits so i need some advice.
Literally everything i've tried doesnt work. gwizard settings, calling manufacture (amana) trial and error, youtube videos, etc.

Machine: cncrouterparts 24x48
Spinde: Bosch 1617
Mods: precision bit collet
Material thickness: .040-.050
Bit: all the bit's i've use are 1/8 diameter and 1 flute (o flute (amana and ebay brand), kyocera single endmill)
Coolant- I've used wd40 but im trying to avoid coolant since im still on a mdf bed- and from my understanding .040 is thin enough where coolant isnt needed (judging from what i've seen on youtube and other threads)
Hold down- double sided tape (forgot which kind but found it on the site- not the sticky gooey carpet tape)

From what I've gathered, it isnt uncommon for DOC: .125 so I've been using .040 figuring that is "safe"
IPM i've tried 20-90
RPMs 8000-2400

I've used these/amana with some success @ 30IPM, ~ 14000 rpm .040-.050 DOC I did manage to get a bunch of cuts at this setting with no coolant and nice chips
Attachment 240818

The Kyocera bits i just got. I have yet to successfully cut anything from them. i've tried 30ipm at 13500rpm, 60ipm @ 24000rpm etc. i have not had "chips" with these bits, it just gums like crazy. I was under the assumption a lot of people use this bit for aluminum since i read it was recommend to buy from "drillman1" on ebay.. any suggestions?
Attachment 240820

And these I have on order- Figured I tried 2 flute since i've only experimented with 1..
Attachment 240822

Any suggestions would be great. Like I said I used the trial of g-wizard and all those setting resulted in broken bits... I have to be missing something.... I've already broken 35+ bits and cant justify buying anymore amana bits at $30+ a pop only to break.. (broken about 8 already including 2 $50 1/4 bits that broke IMMEDIATELY after using the settings the tech told me..... which is why i rather not use amana bits)

[osphoto]

Type of aluminum?

If gummy as in the aluminum is liquefying and sticking to your bits and causing breaks, you are not getting the chips out of the way fast enough. USE compressed air or liquid if not both.

School of hard knocks for me:
1. Unless it's wood: (even then I some times use it) I'm running my compressor to blow chips out of the path and also help keep the area cool.
2. I keep a bottle of WD40 to also help keep things running smoother.
3. If I'm breaking bits at the cutting edge, I slow the IPM. If I'm breaking bits above the cutter edge, I speed up the RPM's. And If I'm at the limit of each and my comfort (aka $) zone, I slow IMP down regardless.
4. If I've done all this and bits are still breaking, I check for run out, clean my bit holder.

Go here:PreciseBits.com Reference Library

I use 1/8 2 flute bits for 90% of my aluminum cutting.



Hope this helps.

[ger21]

I'd use a downcut bit on thin sheet like that, as upcuts will left the material. Make sure you cut all the way through in one pass with a downcut.

The double sided tape might be part of the problem. If the sheet moves even a very small amount, it'll snap the bit instantly.

[muibubbles]

Type of aluminum?

If gummy as in the aluminum is liquefying and sticking to your bits and causing breaks, you are not getting the chips out of the way fast enough. USE compressed air or liquid if not both.

School of hard knocks for me:
1. Unless it's wood: (even then I some times use it) I'm running my compressor to blow chips out of the path and also help keep the area cool.
2. I keep a bottle of WD40 to also help keep things running smoother.
3. If I'm breaking bits at the cutting edge, I slow the IPM. If I'm breaking bits above the cutter edge, I speed up the RPM's. And If I'm at the limit of each and my comfort (aka $) zone, I slow IMP down regardless.
4. If I've done all this and bits are still breaking, I check for run out, clean my bit holder.

Go here:PreciseBits.com Reference Library

I use 1/8 2 flute bits for 90% of my aluminum cutting.



Hope this helps.

I think there are too many videos without coolant (ie toolstoday's video on the amana bit) cutting thicker aluminum that i think .040 should be fine without coolant/air... i'll hook up some compressed air...

what settings are you usings with the 1/8 2 flute bit?

[muibubbles]

I'd use a downcut bit on thin sheet like that, as upcuts will left the material. Make sure you cut all the way through in one pass with a downcut.

The double sided tape might be part of the problem. If the sheet moves even a very small amount, it'll snap the bit instantly.

which downcut bit are you using/recommend? I've gone crazy and im just ordering a ton of bits that "other" people have used with success hahaha

Majority of my work will be .040-.050 aluminum at this time btw..

Thanks!

[alan_3301]

what kind of aluminum are you cutting? I think that is the big question of this thread.

[mcphill]

Have you measured the runout of your spindle at the distance from the collet that you are cutting? Runout will kill small bits on routers, and some routers are just "bad" regardless of the collet used.

[muibubbles]

what kind of aluminum are you cutting? I think that is the big question of this thread.

various aluminum. the 3003 and 3105 are the ones that im really struggling on. the other stuff that cuts well, I'm unsure of. Probably 5000/6000 series

- - - Updated - - -

Have you measured the runout of your spindle at the distance from the collet that you are cutting? Runout will kill small bits on routers, and some routers are just "bad" regardless of the collet used.

im not sure, ill have to check it.

[muibubbles]

Ok, so now im REALLY going insane. I don't understand what I'm doing wrong. literally EVERYTIME I've use some sort of calculator, it breaks my bit instantly. From what I understand, I'm still using settings on the conservative side. 30ipm, .47 DOC and RPM's ranging around 15,000rpms. I'm now running compressed air as well.

I just dont get how manufactures, other sites, and videos i've seen have people running 60-90ipm with DOC .125, 18-24k rpms, with a 1/8 bit...... Considering my settings I would think i shouldnt have a problem at all??

I just used a kodiak 1/8 2 flute zirconium nitride coated bit and cut through 3105 alum @ 30ipm, ~13,000 rpm, .04 DOC perfect. loaded the next sheet and it gummed up and snapped the bit in 30 seconds.... I though maybe it was dull? loaded the new one and it gummed up right away... literally same settings, same material (off cut off the first sheet) brand new bit broken again.

I'm really out of ideas. any help would mean a lot as I'm going broke and really getting discouraged. I'm almost tempted to buy a spindle praying that will solve all my problems........

[awerby]

A real spindle would probably help. They have a lot less runout than hand routers designed for cutting wood, which could be part of your problem. If you've been breaking bits inside your collets, you need to replace the collets, since that damages them. But a new spindle won't necessarily solve your all your problems. There are several other factors involved:

Holding down your material: Thin sheet material can flex easily, so it's necessary to hold it down firmly, since having the material shift or ride up on the cutter is a sure way to break bits. Pros use vacuum to hold sheet down; you might consider that. Double-stick tape can work in some situations, but it doesn't sound like yours is one of them.

The material itself: aluminum comes in different alloys and hardnesses achieved by heat-treatment. Counter-intuitive though it may seem, harder is better and softer is worse, since the softer grades are gummy and will stick to the cutter, especially if you don't use any lubricant. Forget about saving your spoil-board, or use something else besides MDF - at $30 a pop, the bits are a lot more expensive. Inspect your cutters (or the pieces of them left after they break). If they show aluminum that seems to be welded to them, that would certainly account for the breakage. Keep the cut lubricated - with WD-40 or whatever - and brush away any accumulated chips, since recutting chips is not good for the cut or the cutter.

Feeds, speeds and DOC: The charts that are used to figure this stuff out are based on cutting with large heavy-duty mills designed for metal machining, not routers. Using a router to cut aluminum is marginal at best, Only the most rigid and heavy routers are suitable for this. If you're trying to use a router to cut aluminum, then you need to seriously de-rate the settings, by at least half. You might try a lighter depth of cut too - if you take this as a two-step operation, and leave just a foil-thick layer to cut through on the second step, you're less likely to have the material riding up on the cutter and breaking it.

The cutters: While carbide endmills will last longer without getting dull, that doesn't seem to be your problem right now. Carbide is also quite brittle. You might have better luck with HSS or cobalt steel cutters, which are less hard but more flexible. They are also cheaper. Get ones that are short - stub length, with a minimum depth of cut, since the fluted portion is weakest and most likely to break. Flat cutters with radiused corners are also less likely to get stuck in the material.

[ger21]

Can you post some pictures of your broken bits?

[muibubbles]

Awerby, First off great advice! I figured out my recipe to cutting soft malleable aluminum such as the 3000 series! I'm going to try breaking this down as best as I can, you've touched upon a good deal of my issues.

Ger21- I dont have any pictures of the bits as I threw them out immediately out of frustration lol

A real spindle would probably help. They have a lot less runout than hand routers designed for cutting wood, which could be part of your problem. If you've been breaking bits inside your collets, you need to replace the collets, since that damages them. But a new spindle won't necessarily solve your all your problems. There are several other factors involved:

Most of my bits have broken on the cutting side, however last night i broke 2 in the collet. I looked at it when I was changing the bit and was wondering if I should replace it, I'm glad you brought that up! However, it's still very usable for me since 95% of the stuff im cutting is profile cuts in thin sheet metal < 0.050" where edge tolerances is not an issue (as long as the cut is clean)

Holding down your material: Thin sheet material can flex easily, so it's necessary to hold it down firmly, since having the material shift or ride up on the cutter is a sure way to break bits. Pros use vacuum to hold sheet down; you might consider that. Double-stick tape can work in some situations, but it doesn't sound like yours is one of them.

Bingo. Much like working with composites (fiberglass and carbon fiber) there are consumables that come with the job, I always try to minimize my waste and try keeping cost low, wrong. Both labors are pretty pricey-- these are not processes you do not want to pinch pennies-- it will cost you in the end. Essentially I dont think I was applying enough tape. Now, I try and place my 2" tape along the cut lines leaving about 1" on each side of the cut once its cut (holding down the piece, and the scrap) I also tape along the whole perimeter now, instead of ever foot or so.

The material itself: aluminum comes in different alloys and hardnesses achieved by heat-treatment. Counter-intuitive though it may seem, harder is better and softer is worse, since the softer grades are gummy and will stick to the cutter, especially if you don't use any lubricant. Forget about saving your spoil-board, or use something else besides MDF - at $30 a pop, the bits are a lot more expensive. Inspect your cutters (or the pieces of them left after they break). If they show aluminum that seems to be welded to them, that would certainly account for the breakage. Keep the cut lubricated - with WD-40 or whatever - and brush away any accumulated chips, since recutting chips is not good for the cut or the cutter.

Yes- this is something I had just learned in my endeavors with cnc cutting. Luckily when I started I was using higher grade aluminum, maybe 6061? not sure, but once it was dialed in, it would cut well. But not that im using pre-finished aluminum, which only comes in 3000seriees grade (from my supplier) which is softer and caused 95% of all my problems. Now the next foreseeable issue I have will be the spoiler board getting saturated with the coolant and releasing the tape prematurely resulting in shifting part and messed up parts. I'm assuming skimming the top layer of the MDF spoiler board will work? Only issue is I am cutting in my basement and would prefer to avoid mdf dust everywhere Is there another cost effective option for a spoiler board that is resistant to coolant/liquid? I was planning on doing a MDF style vacuum table as my next upgrade but the coolant will be an issue. Any suggestions for what to use?

Feeds, speeds and DOC: The charts that are used to figure this stuff out are based on cutting with large heavy-duty mills designed for metal machining, not routers. Using a router to cut aluminum is marginal at best, Only the most rigid and heavy routers are suitable for this. If you're trying to use a router to cut aluminum, then you need to seriously de-rate the settings, by at least half. You might try a lighter depth of cut too - if you take this as a two-step operation, and leave just a foil-thick layer to cut through on the second step, you're less likely to have the material riding up on the cutter and breaking it.

Hmm, I wish I knew that before. It seemed like all these calculators were designed for cnc router cutting.

So my main issue was my lack of knowledge. I was basing too many things on what I saw on youtube. I've been so hesitant to use coolant because I've seen so many successfully cut aluminum with just air and I was concerned about saturating my spoiler board. But, as mentioned before, there are various grades of aluminum that play a HUGE factor in your recipe. For softer aluminum coolant is a M-U-S-T.

My success came with:

CNC:
2448 cncrouterparts NEMA 23, Gecko G540
MDF bed + MDF spoiler board

"Spindle"
Router bosch 1617 with percision bits collet system cutting at 13,500rpm (speed 3)
1/8" Kyocera single flute end mill from ebay user drillman1
DOC: .050
24 IPM

Coolant:
Air pressure set at 20 psi
Fog Buster coolant system with the nozzle turned about half way open. (slightly more then just a mist)
The coolant I'm using is a sample I received with my Fog buster called S-500 CF Link: Coolant Concentrates | Hangsterfer's Laboratories

Hold down:
JVCC DCP-01 Double Coated Crepe Paper Tape (Rubber Adhesive)
JVCC DCP-01 Double Coated Crepe Paper Tape (Rubber Adhesive) at FindTape.com

Note, with these settings I've made cuts of about 600" with perfect success. I have tried increasing my IPM to 27 and it started welding the aluminum so I believe 24IPM is the max -- which is fine for me. Coolant is spot on as well, any less than 1/2 turn open, it begins to weld. Air pressure is the only variable that could probably adjusted. You may be able to go lower to maybe 15psi, but i dont care enough to gamble with that -- since the air is free =)

[ger21]

Using tape for hold down is probably your biggest issue. The slightest movement of the workpiece can result in a broken bit. If the workpiece moves, it gets pulled into the bit, momentarily increasing chipload by a huge margin.

Also, if a bit breaks in the collet, the chance of another breaking in the collet goes up a lot. Any burrs in the collet will cause uneven clamping pressure, which can cause broken bits.

[muibubbles]

Using tape for hold down is probably your biggest issue. The slightest movement of the workpiece can result in a broken bit. If the workpiece moves, it gets pulled into the bit, momentarily increasing chipload by a huge margin.

Also, if a bit breaks in the collet, the chance of another breaking in the collet goes up a lot. Any burrs in the collet will cause uneven clamping pressure, which can cause broken bits.

Now that I increased the amount of tape i apply its helped out a great deal. I shear most my material slightly bigger than my cut piece so theres not much room to clamp (plus its hard to clamped the inner piece without doing multiple sessions/pausing the cut to move clamps/screws... Do you have a preferred method for cutting thin sheet metal? 95% of my cutting is .040-.050 aluminum.... any milling i do, i clamp.

good tips about the collet, all the info you guys have posted in regards to the collet is very helpful. only thing that sucks is precise bits has a minimum of $50 purchase order >:O And each is $30! I wish I bought a kit with more variety from the start... Is there another company that sells collets compatible with percise bits for cheaper?

[ger21]

Do you have a preferred method for cutting thin sheet metal?

Glue it to an MDF substrate with a light spray of contact cement, and remove with lacquer thinner. It's a bit messy, but it works.

[nlancaster]

I use 3m Super 77 spray adhesive on a nice clean piece of MDF. The aluminum peels right off, and then a bit of goof off to take the Super 77 off.

First piece of aluminum I ever cut on my joescnc 2006 MDF built router. That was a 1/4in downcut at 28k RPM at 30ipm. Now I am building a CNCrouterparts CRP4848
There is a bit of chatter in a few places. But otherwise it is super smooth.

[muibubbles]

with the method of spray adheasive/super77 is the spoiler board reusable? how many times can you use it before junk and chips start sticking on it?

[tony978]

Take a look at mitee grip or per drill pockets an screw down .
Ps use hight speed paths with 10-25% the cutter dia . Full engagement with small endmills never last with the series your using . Last but not least the only machining I have seen that works milling alum at high rpm is daytron with alcohol .

[nlancaster]

The spoiler board is pretty ruined after the lubricant gets on it. So use MDF and throw it away after a use or 2 is hwat I have been doing. Sometimes you can surface it but that only lasts one more time. The hard face of fresh MDF is best to stick too. It might work if you use something with laminate on it. or a piece of plastic that you can clean that the lubricant, in my case WD40, doesnt soak into. I will have to try that next time I do aluminum sheet.

[tony978]

Two prices of cast acrylic with the alum sandwiched precut this top pice windows


Tony

Sent from my iPhone using Tapatalk