Cutting aluminum / Steel

[prosigns]

4737

This is a shock mount/4 Link support bracket assembly t I cut out of a 1'' aluminum plate on the shop bot. I was impressed by the accuracy. It cut cool and w/no shatter. I have a Perske spindle mounted to the shopbot, so I can slow the bit way down

.
4738.

This is the assembly polished and installed in the chassis. I am now cutting the 4 link brackets out of 3/16'' steel plate

.
4739

This is a fiberboard prototype I cut out and bolted up to make sure all the holes (26 in all ) all line up properly. It is cutting (All be it very slow) using a 4 flute 1/4'' end mill bit. I'm very surprised to see it handle the steel job. It is also cutting cool, w/no shatter. I'm very excited about that because I have many CNC part ideas for this project. (A 1970 Camaro Pro Street Chassis).

[Brady Watson]

LQQks great!

What feeds and speeds did you use? What geometry bit for the AL? What RPM did you set your spindle? Cooling/Mister? I have a Colombo 5HP was thinking about trying AL.

-Brady

[harold_weber]

I have Perske spindles, but I'm afraid to slow them down too much for fear that they will overheat (they have shaft-driven-fans). How is your variable frequency drive set up in terms of torque - is it keeping the torque constant at low speeds?

[Brad (Unregistered Guest)]

How long did it take to cut the aluminum piece? Which Perske are you using?

[prosigns]

This is the first parts I've cut aluminum or steel on the Shopbot, so I'm still experimenting. The aluminum I cut about .005" per pass at .005 travel speed with only air blowing on the cut to keep chips out of the groove (Dry). I have a perske spindle and it has a dial control for speed. It has a range from 40 Hz to 300 Hz. I run about 55 to 60 Hz. don't know what that is in RPM, I would guess about the speed of a hand drill? That was with a 2 flute carbide bit. I think I can bump up the speed up some with the 4 flute end mill bit I have now. (Using 1/4" bit ). To cut the steel I am taking .003" passes at around .004 travel speed. and about 60-65 Hz. spindle speed. Every operation I did I bumped the travel speed up a little started at .001 travel speed. I think I can go faster on the steel too. I don;t think I can go much deep per past though, If I go too deep the bit tries to walk on the material - Then I break the bit. Coolant for the steel I used cutting oil. At this point I'm open to any suggestions. This method is producing very accurate, clean parts but it's very slow going. If I can do something different to go faster without sacrificing part quality or damage to the machine I'll try it. Right now at these speeds both the aluminum and the steel are making a smooth cut and the tool and parts are staying cool.


4740
This is the start of cutting the 4 link bracket from steel


4741
This is the inverter for the Perske. I can run the Perske for hours on low speed and it barely gets warm to the touch.


4742
This is the first of (4) four link brackets bolted in place to make sure everything fits properly. The bolt pattern (8 Bolts, every other hole in the aluminum spacer ring) for the bell axle was my main concern. The holes have to be very close tollerence, so the Bracket and housing don't shift under load. Even though the bolts fit snug in the bracket holes the pattern is so close I can tighten them by hand! This bracket has (26) holes in it of various shapes and sizes. It took about 12 hours to cut the holes and another 8 to cut the outline. VERY slow I know, but I'm determined to make these parts in house. The four link bracket came out just as smooth as the laser cut brackets I used on the chassis side of the four link set up. I'm using a modualr aluminum rear end, so there aren't 4 link brackets available in the configuation I am looking for.

[prosigns]

The aluminum was almost as slow as the steel. I think I can improve on the speed. I'm just starting out cautious so I don't break something. It looks like the secret is spinle speed control and a spindle with good bearings so it doesn't shatter. The shopbot itself seems to be up up to the task.

[Brady Watson]

Prosigns (Don't know your 1st name)

To calculate RPM from Frequency, multiply the frequency value X 60. For instance, 55Hz X 60 is 3300 RPM. There should be a function on your freq drive to view output as RPM. My Delta/Colombo defaults to Hz, but I hit a few buttons and it shows RPM. Helps me to minimize confusion!

Looks really good! Keep it up. I have a SB Plasma rig too...it won't mill, but it cut steel like butter


-Brady

[prosigns]

Gary

[prosigns]

Brady
Do you know if there are 3/8" collets available for the perske? I have a bunch of 3/8" endmills I bought on EBAY in a lot that had 4 or 5 - 1/4'' and 1/2'' endmills in it. It woulf be great if I could use the 3/8" bits too.
Thanks
Gary

[Brady Watson]

My Colombo uses ER style collets. Not sure what the Perske takes. What HP one are you using? This place is just one that sells the 3/8 ER type collets: http://www.carolinatools.com/productpages/collets.html

[harold_weber]

Gary, when you say you cut aluminum at .005 travel speed, do you mean .005 inches per second?

Regarding the Perske collets, I know you can buy them at crpindustries.com

You may be able to get a better price at techniksusa.com

If someone else has a good source for Perske collets, please let us know. CRP industries wanted $80 for a 1/2 inch collet the last time I bought one.

[ckurak]

Harold,

Try http://www.woodworkerswholesale.com/. It's run by Thermwood. Mouse over "Collets + Covernuts," then click on "Individual Collets."

They have a number of collets for $35.

I have NOT purchased any collets from them, so you are on your own there.

Charles

[prosigns]

Harold
.005 is where I'm running it now. I only have 1 endmill. I have more coming. When they get here I will speed it up to see how fast I can go. This endmill is no doubt getting dull. I ran .06 on aluminum with no problem.

Charles
I'm going to check out Woodworkerswholesale for the collet. A little bigger (3/8) bit may cut faster since it's stronger. Althought, I tried a 1/2" endmill and it took off as soon as it touhed the surface. Takes too big a bite i guess.
gary

[harold_weber]

The following web page gives the external dimensions on the Perske collets:
http://www.techniksusa.com/wood/din6388.htm
My Perske spindles don't take ER type collets, they take DIN 6388 collets
TECHNIKSUSA just sold me a 3/8 inch collet for my spindle for $36.00

[prosigns]

I received the new end mills today. WOW, I didn't realize how dull the old one was until I installed a new one. Cutting depth went from .003 to .006 and travel speed went from .005 to a blistering .1. What took an hour now takes about 15 min. I tried faster cut speeds and deeper cuts, but I started getting hot chips off the bit. So I backed it off some to save the endmill. I can live with this. I'll post a picture later.

[fitz943]

I don't know if speed is an issue with you, but I run Belin carbide bits at 5/8"-3/4" a second with a depth of 1/8" in aluminum to hog out and just barely slow it down to do a clean pass. I cut aluminum all of the time. I do use a mister though.

[stevem]

Tom, are you using thw Shopbot for your aluminum cutting at those depths?

[prosigns]

Time isn't a real issue when it comes to aluminum and steel cutting. I just do that for the Camaro project for myself, when I don't have any signs to rout.

I havn't used the new (Sharp) end mill on the aluminum yet, so I'm not sure what speed I'll be able to run. Even with the old bit, I was able to cut fairly fast. I'm only using 1/4" end mills. I want the inside corners to be as sharp as possible. Again, speed isn't that big a deal for this project.

I did cut a 1/4" thick aluminum sign face for a lighted sign once in a single pass. Had no problems.

[fitz943]

Steve, I use a 60"x144" Shopbot. I only have a Porter Cable router and I run it on the middle 3 speeds depending on what the bit sounds like.

[prosigns]

4743
4744
4745

I've got the 4 link brackets finished. As you can see from the earlier post I had to redesign the bracket a little. Moved the top wheelie bar mount forward. Added a support tube Between the 4 link brackets at the top with CNC bracket to bolt it in place. Now I can weld CNC tabs to that tube between the shocks (So the top wheelie bar will clear the frame rails). Tube will also be used to mount anti-Roll bar. Still have many parts to make , but I am making progress, It's slow going, but the results are well worth the wait.. The shopbot is allowing me to make all these pro street parts in house. I'm having too much fun.

[gtchea]

Wanting to cut out letters in 1/8" aluminum sheet. What is the best bit to use and at what RPM.

[pappy]

I cut it with a 1/8 inch HSS single flute bit.
The HSS bit is more flexible (vice the carbide which is more rigid and brittle) and you get less breakage that way. You must also run the router on the slowest speed and keep the feed rate down.
Too fast and the aluminum will melt right onto the bit. Additionally you must cool the bit as it cuts either with soapy water or with a "Cool Tool".

[prosigns]

I cut aluminum dry, however with the Perke I can run very low RPM. I try to keep it around 2500 to 3000 RPM. I judge cut speed by how it sounds and if I'm getting nice clean chips off the bit. I used a 4 flute spiral up carbide on 1" thick aluminum and only had to lightly sand the edge before polishing.

[the_whaley]

One suggestion, I have been a tool maker for more than 20 yrs. A couple of the things I would do to improve cutting time. A. use a coolant, you can buy over the counter stuff like cooltool at industrial supply houses, but try some kerosene, its cheap and works great. B. reduce the amount of material to go per pass. For an example, if you use a drill pattern with an endmill, drill holes connecting the dots around the profile of your part. Space the dia so the holes over lap themselves. (the end of the end mill will remove the metal in an upward direction) and will remove it so much quicker than conventional milling. You may have to adjust the offset to make sure the drill pattern doesnt wobble into the finish outline. This method will allow you to remove the bulk of the material and you can go straight to finishing cuts. With the use of kero you should be able to take full cuts to depth and at least .030 per pass ,depending on your set up. It is entirely feasible to drill your pattern with strategically place short z passes to leave tabs a one pass finish cut, cutting tabs and all. Good luck some really nice stuff you have there. Ps. be sure to use a two flute center cut high helix endmill.

[dingwall]

I just did a part for my mountain bike. I'm really impressed with how it turned out. I'm not sure if it was the new Bosch router, or new endmill with cutter geometry designed for aluminum, but it worked really well.

4746

[alano]

Sheldon,
Wow! Nice job!

Curious, what are the details on the special alum end mill. Also, what feed rates and depth per pass did you take? I'm assuming this is 6000 series aluminum.

Thanks,
Alan

[rookie432]

Sheldon,

I'm interested in these answers as well

[dingwall]

The bit was 1/4" high speed steel with maybe a 45 degree spiral. I basically just asked for an aluminium specific center cutting endmill at the local machine shop supply house. I applied constant squirts of water based coolant with one hand and occasional bursts of compressed air with the other to clear chips. I have a steel table bed, if it was wood, laying down some plastic sheet would be a good idea.

I ran the bosch at top speed 25K, max depth of cut 1/8", feed 1/2"/sec.

I'd spec'd a cut off of 6061 from my supplier, I'm not sure if that's what I got or not.

I've cut aluminum with a carbide routerbit and a Porter Cable 7518 router before and have not been impressed with the edge finish. I assumed I was just asking too much from the bot. The edge finish with this setup is beautiful.

[gerald_d]

Higher up in this thread is a picture of an inverter for a spindle. That inverter is a 0-400Hz TB Wood’s E-trAC WFCHT high torque Series AC Inverter (http://www.tbwoods.com/products.php?level=4&GID=37&PID=31&MID=2). Just something I'd like to record here in case I find an old spindle without an inverter one day . . . .

[dingwall]

Gerald, there are a lot of spindles on ebay.

[gerald_d]

Sheldon, I live 5000 miles away from ebay

[waynelocke]

Has anyone purchased one of the spindles on ebay and added an inverter. How hard is it+
Wayne Locke

[Brady Watson]

Wayne,
If the spindle is 3 phase, you will need a phase convertor if you are only running 1 phase in your shop.

After you have 3-phase ready to go, you need a high frequency invertor to control the spindle speed. I have a Delta Hi-Freq running my 5HP Colombo...and already had 3-phase in my shop.

You need 3-phase to the invertor and then power and signal wires to the spindle. From what I understand to replace the bundle of power and signal wires on my Colombo to the freq box is like $500...not cheap.


-Brady

[gerald_d]

There are inverters that will take single phase in, and produce variable high frequency three phase out. Example (http://www.ekstromcarlson.com/frequency%20drives.htm)

[K. Simmerer (Unregistered Guest)]

Sam,
In case you thought no one was listening "thank's for the tips". I always appreciate an experienced hands better way to skin the same cat. Makes a lot of sense!

[Brady Watson]

That makes sense Gerald. Nice find!

-Brady

[gerald_d]

Brady, those Ekstrom-Carlson inverters I spotted above are actually produced by Leeson (http://www.leeson.com).

[jthelen]

Sheldon,
Did I understand you correctly. You cut aluminum at an RPM of 25K, max depth of cut 1/8", feed 1/2"/sec.

My table top is T-6 aluminum (6061) 1 inch thick. I cut the channels for my vacuum system into the top. I use a 3/8 inch bit taking .050 per pass at 4 inches per minute and 10,000 Rpm's. (as slow as my Makita router will go) I cut this dry.

The bit I use was an aluminum cutting bit from Onsrud. http://www.onsrud.com/ I cut a 1/4 inch deep on 1 3/8 centers and a lot of passes. I cut it in 4 quadrants and have about 2 1/2 done. I bought 2 bits for this project but have only use the first one and can't tell the difference in sharpness against the unused one.

I would like to increase the speed and/or depth a little as this takes a long time. What did you bit look like at those feeds and speeds? Did you use a coolent?

Jim

[jthelen]

Sheldon,
Did I understand you correctly. You cut aluminum at an RPM of 25K, max depth of cut 1/8", feed 1/2"/sec.

My table top is T-6 aluminum (6061) 1 inch thick. I cut the channels for my vacuum system into the top. I use a 3/8 inch bit taking .050 per pass at 4 inches per minute and 10,000 Rpm's. (as slow as my Makita router will go) I cut this dry.

The bit I use was an aluminum cutting bit from Onsrud. http://www.onsrud.com/ I cut a 1/4 inch deep on 1 3/8 centers and a lot of passes. I cut it in 4 quadrants and have about 2 1/2 done. I bought 2 bits for this project but have only use the first one and can't tell the difference in sharpness against the unused one.

I would like to increase the speed and/or depth a little as this takes a long time. What did you bit look like at those feeds and speeds?
Jim

[Brady Watson]

Jim,
You will need some kind of coolant for the bit. The easiest would be to mount a magnetic gooseneck and blow compressed air on the bit. Liquid coolants are not really needed for AL.

For feeds and speeds, you mainly want to focus on chipload and sound. It's the chip curl that pulls the heat out of the bit. You want the largest chip your machine can handle without chatter or bogging. If something doesn't sound right, chances are it isn't. Quite a different sound than wood routing. You also want to watch that you don't take off too much at a time and lose steps as a result. Even the alphas loose steps when they are pushed beyond their limits.

If you push things too hard, and break bits, switch to a HSS bit. HS Steel bits are more resilient than carbide and will stay together in the event that you shock the bit. I would recommend ramping into the cut if you decide to go deeper than you already are.

Conversely, you can also break the bit by spinning it too fast and not moving the machine fast enough (too small of a chipload) This causes the bit to heat up and it will break.

Hope that helps,
-Brady

[jthelen]

Brady,
Thanks for the advice. Do HSS bits stay sharp in aluminum?
I forgot to mention I do blow air through a small copper tube at the bit to blow the chips away. I guess it keeps the bit cool too. I would touch the bit as soon as it spun down and it wasn't even very warm.

On another note... If you accidentally double send a message on this forum can you go back in and delete one?

Jim

[Brady Watson]

HSS bits do not stay as sharp as carbide in any material. You give up the advantage of tools staying sharper longer when you move over to HSS, BUT they are substantially cheaper and are less prone to breakage. Carbide is a much harder material than HSS, much like a diamond is harder than lets say a piece of steel. If you hit the diamond with a hammer, it will shatter...the piece of steel will either dent or absorb the shock. Hardness is basically the ability to resist scratching...or in your case, dulling.

Nope...can't go back and delete a double post. You can edit it if you are quick enough to a blank or nearly blank message. Otherwise, one of the monitors will delete it.

-Brady

[gerald_d]

For cutting metals, you need a coolant and a lubricant. The traditional coolant/lubricant used for aluminium is plain old kerosene - look at sam whaley's post just above the picture. Alu. has a habit of sticking to the bit, and the lubricant stops this.

[Brady Watson]

Gerald,
Yes and no...It depends on the hardness of the AL and if you are using the proper speed, feed & RPM. Generally speaking, the harder the AL, the easier it is to cut. Soft AL sticks to the bit and requires lubricant in addition to coolant.

Many bits are designed for cutting AL dry ~ again, it will depend on the factors above.

-Brady

[jthelen]

I used T-6 (6061) because of it's machining properties. I cut some panels for someone once that were soft aluminum and you never seen a better weld then I had following the bit.
Even 6061 will melt if you go too fast. In setting up to cut my top in jog mode, I hit 1 inch instead of .1 inch Z down, I made a new bit into a steel/aluminum rod. To this day I can't get the aluminum out of the bit.

[gerald_d]

Brady, I have yet to meet a metal that cuts better without a lubricant. Sure, there are bits that are supposed to be okay if dry, but they all cut better (and last longer) when they are lubricated.

Jim, the weld that you saw behind your bit is a form of "friction stir welding (http://www.azom.com/details.asp?ArticleID=1170#_Friction_Stir_Welding) "

Merry Xmas all - I'm off to lie on the beach for the silly season around here.

[dingwall]

Jim, I don't do a lot of cutting in aluminum. That's just what I used that time. I used a waterbased coolant/lubricant squirted on with a hand held oiling can. I have an air chiller, but have not used it for aluminum.

Most of the endmills for aluminum are either HSS or Cobalt. I've heard machinists say that carbide doesn't work as well.

[mike_zacur]

just from my experience using the bot to drill holes in .625 aluminum (about 50,000-100,000 per year) i found water using a koolmist sprayer to work well.i used to use a pc router at 10000 rpms with a feed rate of .10 ips. Now i use a columbo spindle at 7200 Rpms with a feed rate of .25 ips. my drill bits usually will last for 10,000 holes before needing replaced. when the spray system fails the drill bit will overheat and the aluminum will melt on the bit within 10 cycles

[dingwall]

How do you keep the koolmist from fogging up the whole shop? I quit using ours because of that.

[Brady Watson]

So...are you guys putting plastic sheeting down underneath your AL parts...or are you letting that coolant/lube soak into the spoilboard???!!!

I like to machine AL dry as much as possible...because I also use my Bot to cut hardwoods. Last thing I want is that juice getting wicked up into a piece of mahogany...OR warping my spoilboard.

What do you guys do?

-Brady

[simon]

Brady

I cut aluminium using Methylated spirits. In case this does not translate to american, it is the purple coloured alcohol favoured by itinerants as a drink.
It is volatile so it evaporates really fast and cools really well. Also it does not do any damage to a spoilboard.
I would not use it for anything but ally, because ally does not create sparks when being machined.
I do not cut ally very much, so I just spray it with a garden mister. You can hear the difference in the noise when it goes dry.
It is also cheap.

[Brady Watson]

Hmmm...Simon...We call that cheap liquor in the US Mad Dog 20/20 (http://www.thedrinksgroup.co.uk/md2020.html)...I knew there was another application for it!!! LOL!

Good tip though...sounds to me like Denatured Alky would work well...I used to use it in my turbo car to cool the intake charge...and run 30#s of boost on 93 octane. It had an vacuum/boost actuated switch on it that would inject alky into the intake from 15 psi & up. Something like that just might be the ticket for machining AL.

-Brady

[dingwall]

Aluminum doesn't spark, but your router brushes do.

Brady, I have a steel table bed. You could throw some melamine over your spoil board to catch the drips.

[paco]

Or machine a "pan" out of polycarbonate or UHMW 1/4-3/8" thick material with a dripping drain to recycle the collant lube... still, depends on the size of the AL sheet/plate to be machine... an idea that I had about this... depends too on the frequency that one machine AL with his tool since a such pan can be worth some $$; but still, can be fast to install and remove in between wooden working!?

[Brady Watson]

I'm lucky in the sense that 2D profile passes can be done on the plasma bot...and then if need be, fixtured above the spoilboard on the router bot with vacuum pods to get a nice crisp shiny edge...Although the plasma has been very good since the change to SB3...but I can't do pocketing and things of that nature on the plasma.

Sheldon, good idea with the melamine.

-Brady

[amorgan]

I see in this post that some are recommending fast speeds cut speeds for aluminum and others slower feed rates. For routing, do I just have to do a lot of experiements (and go through a lot of bits) or is there a better way to optimize the amount of material cut. An example of the cuts I'm tring to do is to round the end of a 4" x 3/8" aluminum plate. It seems like it depends a lot on the individual bits.

I'm using a PC router.

Andrew

[Brady Watson]

Andrew,
Note that Gary has a spindle and is able to turn his RPM way down...so your PC @ it's lowest setting will be 10,000 RPM.

The main issue with cutting AL is obviously heat. I would start at .8 IPS at 10k RPM with a .02 stepdown. See how that works. Get a squirt bottle with soapy water in it or use coolant recommended for AL...or rig up a compressed air nozzle on the bit to air cool it. The main thing that you are looking for is welded chips on the top edge of the piece. You should be using an upcut spiral with a high-helix angle for cutting AL. If the top edge is smeared up over the top of the piece, it is getting too hot and you need in increase move speed.

Play around with depth of cut and move speed until you get a nice edge and good chip extraction. Heat is the issue...tools will last a good amount of time if you keep the heat at bay. I quite often cut AL on the miter box and if I spray the blade down with WD40 now and then, things are good. If I don't it welds the AL chips to the carbide from frictional heat...same thing to watch out for with routing AL.

Hope that helps...don't feel bad if it doesn't work the 1st, 2nd or 3rd try...keep trying, you'll get it dialed in perfectly. Oh, and be sure to write down what speeds, stepdown and RPM you finally go with so that you don't forget!!!

To bolster your confidence, have a look at this video (http://www.cncmotion.com/aluminum.mpg) be sure to turn up your sound so that you can get an idea of how things 'could' sound. Note the depth of cut and how aggrsively they are moving thru the material...mainly note the nice big chips coming off of the bit.

-Brady

[amorgan]

Thanks for the help on this. It seems counter intuitive, but cutting faster (to a point) makes a better cut. As you pointed out, the trick is getting the right chip load (a combination of rotational speed and feed rate). With the PC router, we found the best cut at 19,000 RMP and 3 ips with a two flute 1/2 in bit. However, we had to take a very small cut (.020) otherwise the router bogged down. That was also the problem when we slowed the speed down to 10K. As soon as it took a cut, it would bog down. We're trying to cut a radius on a piece of 4" wide 1/4" bar stock and it takes quite a while at .020 per pass, even at 3 ips.

One problem we are seeing is that even the best cut on the radius isn’t very smooth. Taking a thin surfacing cut at the settings above, the cut looks really good, but off the side of the bit, the cut is pretty rough. We tried taking very light passes at various feed rates, but couldn’t seem to find anything that worked really well. I haven’t tried to measure the run-out on the router yet (didn’t have the gauge handy), but it is nearly new, so hopefully the bearings are not a problem. I don’t know if this is because of the router, the material or the ShopBot.

Most of my experience is using routers on woodworking and up until now, our experience with aluminum has been mostly with a saw, plasma torch and welding. This is our first foray into CNC with aluminum, so we have some learning to do. The good news is that even with the limitations in cut speed, just by automating the drilling of holes and a few routing patterns, the ShopBot is going to pay for itself in just a couple of big jobs.

From what I’ve learned and read on this forum, it looks like we are going to be in the market for a spindle. Given what we are doing – mostly cutting aluminum, would a 3hp spindle be enough or do we need to just take the plunge and get the 5hp. Right now, the router is clearly the weak link. At what point does a larger spindle become ineffective because it is more than the frame of the ShopBot can handle? Is the 5hp spindle at this level, or could a ShopBot handle more before the frame flex becomes the weak link?

Is this something that is best to buy directly from ShopBot to get the bracket and other pieces (what else would we need?) to move from router to spindle, or is there another place that has a better deal on spindles? How much should we expect to pay to upgrade to a 3 or 5 hp spindle?

Thanks,
Andrew

[paco]

Hi all!

thought I post some of my first tests...

This is 3/16" thick... soft in front... hard AL is the one standing on the edge...

4747

lub in soft AL is kinda a better!

4748

Once more confident...

4749


4750

Thoses are from a PC7518; could be better I believe... though acceptable...
0.3-0.5"/sec., 10 000 (hard AL) - 13 000 (soft AL)RPM, 0.020" stepdown, WD-40 lub; does'nt need much; hard AL could be machined without lub but better finish with... used a specific 1/4 CED AL endmill 2 flutes... look like...

4751
still in a very good shape even after some quite severe tests I made it go through!!

[Brady Watson]

Looks pretty good, Paco. How did you hold the parts down? I think that the lines on the parts are the result of vibration and deflection.

What's kind of strange is, hard AL usually machines better than 'soft' AL. 6061-T6 is a great alloy for machining...not sure what you are using here.

One thing that is deceiving when machining AL on the bot, is the sound. Machining AL is pretty loud due to the vibration being transferred to the machine. Usually the softer materials like wood & plastic absorb this sound...and if there is a problem, you know it right away. When machining AL the sound is so strong that it is hard to get the speed right by using just your ear...if you know what I mean. Running AL on the router just 'sounds' wrong at any speed. Take a look at the link I posted up this thread...turn up your sound and you'll see what I mean.

-Brady

[paco]

Brady,

I use clamps with tabs. I believe thoses vibrations are from the PC runout combine with it's lack of a good RPM control... and the fact that I used a 1/4"CED tool... faster than 0.5"/sec. at 10 000- 13 000 RPM, I could feel the chattering (and hear) on the router body... but never on the AL blank...

I found (so far) that soft (utility) AL need to be machined at a faster RPM (13 000) than hard AL (10 000)... most of the scrap piece of thick AL I have (3/8" or more) are either T6 or T7... I've been told in the past that 3/8" thick or more AL are "always" hard AL...? This 0.5" test is with T6...

I've download this video and was really impressed by the aggressivity with which "they" machine; I think both machine stiffness and spindle setup play a great role in this achievement... and it look like "they" use a somewhat large cutter (3/8" - 1/2" ???)... The sound I got was OK the way I feel it... but sure different than woods or plastics...

I'll be ordering new tools today... more later...

[Brady Watson]

When you order your new tools, tell them to throw in a Colombo while they're at it


Yes...I even think that the cutter they are using is more like 1" in diameter...with quite a bite of material taken off in one pass. Looks to me like they are down a good .125" or so.

-Brady

[stevem]

Cut in 6061-T6 with Makita RF1101.
Roughing pass with .375” flat router bit, .100" step down, 65% step over, 16,000 rpm at 10 IPM.
Finishing pass with .25” ball mill, .010” depth, 3% step over, 19,000 rpm at 60 IPM.
Light sanding with 220 grit wet paper.
Total depth: 1.010"


4752

[paco]

Very interesting Steve!

When you wrote "flat router bit"; what is it exactly?... straight edge carbide tiped?... or was it a wood router bit or a AL spec. spiral up router bit?... how many flute?... I've been told that 3 flutes would do a better finish...?

Slower than what I did (about half the speed I used)... but what a bite (0.100" step down; that's five time the setting I used)!!!
Hummm... from your finishing pass; I wonder if I would gain in total time with 0.010" step down at 1"/sec.?!?!?

Bigger tool are sure stiffer... but I'm always tend toward smaller ones...

[stevem]

Paco,

Flat, bottom cutting, straight flute, carbide wood cutting bit. Two flute. Not worried about finish on a roughing pass. The ball mill is solid caribde with 4 flutes.

[gerald_d]

Steve, you do know that you are not allowed to get that finish with a humble router - are you sure that you didn't use a spindle?

[mikejohn]

naughty,naughty!!

[gerald_d]

[paco]

Thanks for the info Steve.

I've been suggest to try 2 edges straight carbide tiped wood router bit but I was kinda suspicious about thoses...

More curious; did you used lub or coolant? What about your plunge speed?

I had to plunge quite carefully/slowly but did'nt get much improvments from ramped plunge...

[dingwall]

I'm currious about cutting dry too. In Brady's video, they are obviously cutting dry, but they also have a spindle with presumably way more power than a PC and also the machine looks to be a lot beefier than the SB.

So my question is, is it possible to cut 6061 dry on the Shopbot with a PC router?

[paco]

Hi Sheldon!

You can but the lub will help on the finish; less or no burr and cut edge cleaner (no powdery rewelding)...

Here what I got in 6061-T6 cut dry...

4753

[Brady Watson]

Another option is to use compressed air and a nozzle pointed at the bit as a coolant. Although a standard nozzle works fine, you can also cool things down a little more with a vortex cooler as well.

-Brady

[paco]

Brady,

I'm not sure about air cooling for burr and this kind of dusty rewelding... but sure worth trying...

Many type of geometry for AL router bit are available... might worth to test some but some are quite expensive... even in small CED bit...

I just tried myself with a 1/8" CED 2 straight edges carbide tiped wood router bit to cut a capital "G" (about 4.5" tall) in 0.090" thick soft AL and it came out as good as my previous tests in thicker AL with 1/4" tool... still need a lub to avoid top burring... I used the same setting as previously: 0.3"/sec. feed, 0.1"/sec. plunge, 0.020" stepdown, some tabs to hold the part to the blank... I was a little shy since this test was with a 7/16" CEL long tool...

More later...

[Brady Watson]

Paco,
How big are the chips coming off of the tool? It seems to me that you need to move faster to avoid the welding/smearing (I know exactly what you are talking about). Be sure to have the AL firmly fastened to the table, and try running same depth of pass, same tool (should be a high-helix angle spiral for AL)...I know milling that fast seems wrong....but try it at .5 to .8 IPS. Be sure to start OFF of the material. Create a stright lead in to avoid the dreaded plunge...and drill a hole in any inside portions/islands so that the bit only has to move XY in the material. You may be suprised at the results of increased speed.

-Brady

[paco]

Brady,

so far, I get "chattering" if I try to push it some more... at 13 000 RPM (soft AL)... I did get up to 0.5"/sec. but the tool eventually "chatter" at some point/direction... slow plunge (0.1-0.2"/sec.) are OK... remember that I've tested 1/8-1/4" CED tool so far; I'm pretty confident that one can push more with bigger tooling... I don't get your suggestion wrongly for sure since most spec. in catalog pretends that one should push up to 3"/sec. with a 1/4" CED tool... at 100% s-t-e-p d-o-w-n!!!... are'nt they selling bit?! ;-)

Though I did, accidently, plunge at jog speed (15"/sec.) in the 0.5" thick T6 (while X&Y jogging too) without breaking the 1/4" CED tool... in fact, I drilled this "steak" through in about a second!!!... and the machine was looking for more!!! 8-D

I plan some more testing about speed soon... just that I kinda don't like breaking new bit... cheap I am!!! 8-)

[Walter Hicks (Unregistered Guest)]

I have a shopbot with a colombo spindle and I'm trying to cut 1/4" 5000 series alum. with a 1/4" carbide bit. I'm finally having decent luck but I'm cutting in 8 passes, 11000 rpm, 2"feed rate. Anyone have a suggestion on something I need to change?

I am also interested in a cold air gun. I have a mister now but it's killing my spoilboard. Where can I find one?

[paco]

Hi Walter!

This is quite a good feed with a decent stepdown! Here a link to "air gun": www.arizonavortex.com/cooltool.htm (http://www.arizonavortex.com/cooltool.htm)
Pics?!

[paco]

Hi all!

Anybody gave a try the 63-600 onsrud serie?... and did they met the advertised specs. (100% stepdown)?!

I'm about to order a bunch (1/8" CED) for a large sign project and since they are quite expensive bits... I'm kinda worried about bit breakage issue since I've breaked a couple 1/8" CED (different type) with only 0.03" stepdown... thoses are advertised to be able to single cut 1/8" thick AL at about 1 to 1.5"/sec.!?!?!?

[wayne_walker]

I would like to cut some 5052-H32 1/8" thick AL. From the above posts, it would appear I should use a 2 flute HSS bit @ 10,000 RPM and cut at .25 IPS using a coolant and lubricate. Is it possible to cut this in 2 passes?

I am using a PC router, so my speed control is limited.

Thanks in advance for any advice.

Wayne

[paco]

Hi Wayne!

I'd say avoid HSS with such RPMs as router motors... you'll burn 'em way too fast.

[jim_staud]

On behalf of Brady watson I am moving his post here for others reference.

Jim,
Have a look at these 2 videos showing AL being cut on a CNC router.

http://www.cronsrud.com/video/special/pages/videos/aluminum_heavy_cut.mov

His Video Link2 was a copy of that provided above by Jim Thelen

Make sure that you turn up the sound so that you can hear what it will sound like...cutting AL sounds 'wrong' compared to most other materials when cutting.

The important thing to note when cutting AL, is that it is very dense compared to wood products. Therefore, it is imperative that you ramp into the cut or lead in from the side, as is shown in these videos. You will also want to keep in mind that you want nice big chips coming off of the part. A common mistake is to run the feedrate too slow, which causes the bit and workpiece to overheat. Compressed air is a good way to cool the bit and keep the AL from 'smearing'. Generally speaking, you want to move quickly thru AL, without slamming the bit into the workpiece...Keep in mind that the stiffness of your machine and how tight it is will influence cut quality.

If you need a baseline for cut speed & chipload, use the new ChipLoad Calc in the SB3 software under Tools. You should ideally use an endmill OR a single flute tool like Onsrud 63-618 or 63-620, and the shortest cutting length that you can get away with. The longer the bit, the more deflection and potential for breakage.

Material hold-down is also critical. You will need to use 2-sided adhesive tape, vacuum or bolt the AL down if necessary. Any movement of the AL will cause unwanted vibration.

There are other factors to think about when cutting AL. One is, what grade AL is it? Most say that 6061 is the best for general machining when speaking of thick (.25" +) parts, since it is harder than some of the other alloys. The harder the AL, the easier it is to cut and the less prone that it is to overheat and 'smear'. AL sheet (thin less than .125") is best machined with a downcut spiral bit to keep the edges from lifting when cutting.

A spreadsheet of feeds & speeds for all materials is a good idea...however, many times what works for you, doesn't work for someone else due to differences in bits, router capabilities, choice (alloy) of AL chosen etc...When trying out new materials (in your case AL) I tend to start out slow and increase the feedrate gradually as I am testing the properties of the material. After a few cuts, I can pretty much get things dialed in to the proper speeds.

Hope that helps,
-Brady

[charles_o]

Jim
I also moved this from the other thread

The spreadsheet or data base would be great if someone could pull it off. Until then some interesting reading and tools about this subject.

http://www.denford.com/Calculate%20Speeds.html
http://www.denford.com/Calculate%20Feeds.html

http://www.plasticrouting.com/BitSearch.asp?Page=Material
http://www.plasticrouting.com/Van.asp
http://www.onsrud.com/popChart.html

Charles

[jim_staud]

Charles,

Have you seen a similar chart for Aluminum cutter selection as the plastic one from Onsrud? The information on their site explained the development of the plastic routers and that the ALuminum Cutters are considered a much simpler application based on limited types of raw stock.

Those first two are very informative. I can easily make an excel spreadsheet to quickly determine a speed and rate from the router speed range and the cutter specs.

Jim

[jim_staud]

Prosigns Gary,

Did you find any good leads on pricing for the Perske Spindles?

Jim

[charles_o]

Jim
I haven't ever found anything for metals as Onsrud has for plastics. When using a material that is new to me, I have found the Denford calculators useful to get close to the right rates and then "tweek" the setup thru trial and error. I also have found building relationships with technically adept sales reps to be a great source of information. A good rep does not want to recomend a product or proceedure that will fail in your application and drive you to the competion.
Good luck

Charles

[woodduck]

Just wondering what everyone is toolpathing with for metal milling. Could you use Partwizard or would you need a more machinist oriented cam software like Millwizard?

[paco]

Hey Scott,

the "major problem" with PW is that it does'nt ramp into start point/entry... else than that, it can do the job... until you decide you need more control. As for ramping, you might find solution like slow plunges (still depends on tool bit type) or manual coding... maybe spiral hole boring (at start point) from the Drill Press (Virtual tool). It's just better to ramp into AL for bit survival... MillWiz will only help you with 3D toolpath for 3D designs. Are you looking for 2D or 3D work here?

[Brady Watson]

Scott,
You can use PW or MW to create your toolpaths for cutting AL. Paco makes some great suggestions. You can also use the Lead In feature on a Profile toolpath to either start at a drilled hole and lead into the profile or, have it lead in off of the material.

Using MW to do 3D, be sure to do the roughing pass and preview it in SB3. The major concern that I would have is the area around the part (the 2D outline of the part) where the bit wants to go full depth. When rastering, the bit will have a tendency to rub the walls of the scrap when rastering. If I were going to cut something 3D in AL, I would 1st cut it in a softer material, like insulation foam or wood & watch for situations that would be a problem when cutting a harder material like AL.

-Brady

[woodduck]

I'm looking for 3d work here, as in an export from Rhino ...mostly small disc shaped parts but 1" thick and with milling of different depths on 3 sides. It sounds like Millwizard would work but is there something better for my purposes?
Thanks

[paco]

Got to see the part(s)... "different depth on 3 sides" does'nt say enought; steps, slopes, flat bottom pockets... screen shots?!

[Brady Watson]

Scott,
The downside of MW is that your toolpaths are confined to a square or rectangular 'bounding box' of the part. If you just want to machine within the confines of the footprint of the disc, then you have to move up to something like ArtCAM or pay someone to create the toolpaths for you.

No problem exporting from Rhino. I would recommend exporting as STL binary format. This will pull right into MW or ArtCAM (and many other CAM packages as well)

If you can post some kind of picture as Paco suggests, we would be able to help you out with more detail.

-Brady

[woodduck]

Here is the part, it has a diameter of 2", a thickness of 1" and various pockets from each side. I hope this shows it enough.
Scott


4754

[woodduck]

Here is another view; note that the weird whale shaped hole and the round hole are pockets (flat bottom). Yes, I will need to machine within the confines of the disc since it will be an end cut from a solid 2" rod.

I haven't bought anything yet as far as a CAM software so I'm open to anything ( just about to order my 'Bot)

I intend to do mostly cabinet parts but also have a need for custom aluminum parts like this. Maybe I'm confused but I thought I might need 2 different CAM packages for the 2 different applications?

Cheers, Scott


4755

[paco]

Scott,

my first question would be; what kind of tolerance do you need on thoses parts?!

My second question would be; just how many of thoses part do you need?!

The "weird whale shaped hole" should'nt be a problem assuming you can use a 1/4" CED tool bit (or if you got plenty of time to allow, a long reach 1/8" CED... maybe you could find a 3/32" CED). But you'll need a "GIG" for this... The other side holes are what would got me a challenge; this would be a nice part to do on the indexer with a hold down that would use the "weird whale shaped hole" as a reference and make the through holes half at a time rotating 180 deg. for each sides. But to slot through 2" thick with a 1/4" CED tool in AL... this will take long... maybe you couls make the side holes first than the "weird whale shaped hole" usine the side holes as reference...

Anyway, to answer (try) your question, I believe (firmly) that's 2D strategie. Hence PW can do the trick just fine until you need more, advancede ramping entry and such.

To cut cabinet parts efficently (to CAD fast enought) you'll soon be looking for a cabinet specific kinda CAD... but PW can do it if you're not in a hurry. As for CAM for cabinet parts, you don't need anything very advanced until you cut a hundred each week... I believe... It's more about saving the CAD part time involved... CAM is usualy fast or it mean you don't use the right package.

Let us know how you achieve to machine thoses parts... I'm curious about how you'll figure...

[woodduck]

Paco and Brady, thanks for the responses, after talking it through with you both I realized what my real question should have been: I will be getting either Artcam/Insignia/Cabinetmaker or Enroute/Wood for my cabinet parts...Can I use either of these for metal milling as well and avoid getting a seperate program for metal work?

Paco, I think the tolerances I need are .003" and I need only 2 of these as a prototype. If it works, then I will probably get a bunch injection molded or cast. I would just like to be able to do these prototypes myself since it's impossible to get someone to even look at a job this small.

Thanks again, Scott

[ron brown]

Hello Scott,

Before you try a package that won't work you might try toolpathing in Rhino and exporting DXF, convert with ShopBot software.

The product I use and many here have tried and failed is Vector. It allows complete control of the toolbit once you learn the interface.

I think one of the problems you will have is indexing and holding. I think I might take a the piece of Aluminum as a Block. Drill and slot the features on the radius side. This will allow you to mill from both sides. The block would then be secured and indexed on the flat side. The "Whale hole" would be milled and then the outside would be cut.

Good Luck,

Ron

[gerald_d]

Chasing a .003 tolerance, in alu, 2" deep, with a ShopBot, for a novice, has a very low chance of success. May I join Ron in suggesting that you use rectangular matrial and wishing you luck? (The software will be the least of your headaches).

Have you considered getting someone to "grow" this part with epoxy/lasers? (Can't think of the right name for this process now)

[paco]

I would start with flat stock too and try to index with the "weird whale shaped hole" for the side work half depth at a time. I think one can achieve quite good tolerance on each seperate toolpath (as accurate as the Bot is...) but the challenge is to accuratly indexe 'em from each other.

Have you consider have 'em quoted on a CNC milling while you provide the CAD part of the project? It may be still quite expensive but fast and as you intended to have 'em.

If you get Cabinet Maker (artCAM) you'll have to get Insignia along, if you get PRO (ArtCAM) you'll have Insignia (as part of the budle features but not Cabinet Maker (maybe you can add it to PRO like add it to Insignia)... There are'nt much feedback about Enroute (I wish there we're more), but I know it's more expensive. With all the feedback you can have about ArtCAM products, I would give a fair chance to Vector (Ron would be there to help!)... If you choose ArtCAM products, my feedback is that you'll have a good feeling in the short run, but as time goes, you will find bugs and missing feature you'll say "should'nt that be there?!?!?" I believe that you'll find a way to do your AL milling in all of 'em just as in PW for basic stuff.

[woodduck]

This does make sense, to use a square block first. it would make it so much easier to keep rigid. Also, Ron, I think Delrin would work just fine so may go that route. I need to finalize the design before I proceed so I may make it easier yet. It sounds like Insignia will work for me but I know I have a lot of learning ahead. Thanks for the help!
Cheers, Scott

[dave@sprut.co.uk]

Hi all, I hope you don't mind me posting this here, but it seems to be 'on topic' for this thread.
I've recently completed a ShopBot postprocessor for one of our customers who is running our SprutCAM software.
The post supports 2D & 3D machining and also peck drilling as well as helical machining of holes (using CG) and profiles .
SprutCAM will accept native Rhino models as well as iges - dxf and eps amongst others.

You can use a default 'workpiece' of box - cylinder or casting, or you can use an imported workpiece model.

It has 2D carve engraving. It also supports various plunge and approach/retract moves for pocketing.

There are two versions available, SprutCAM Expert which is 2 & 3D and SprutCAM Machinist which is 2 & 2.5D.

If anyone is interested in a 30 day trial, let me know.

Thanks for your time.

Dave

[robtown]

.stl ? I didn't see .stl in your list, as well what about .3ds files?

I'd love to have a 30 day trial, I'm about to start a project where I've been asked to create 5 different 3d textures to be routed into panels, an example of one I already did for them is here: www.robtown.com/portfolio (http://www.robtown.com/portfolio) (scroll down to the GA Aquarium section), I'd like to see how your tool stacks up, I did the prototyping on my machine, but the final output was done for KOMO via AlphCam

[dave@sprut.co.uk]

*.stl we can do but not *.3ds.

I will e-mail you shortly with the download information and the ShopBot postprocessor.
The textured wall panels that you did look quite interesting. Are they purely decorative or for some kind of noise insulation?
I have put an image here (http://www.download.sprut.co.uk/Forum_Images/R0010475.JPG) of some of the first parts that my customer created using SolidWorks and SprutCAM.
If you have any questions, I'll be happy to answer them.

Dave

[jim_staud]

Dave P,

Can you explain the SprutCAM vs RhinoCAM (MillWorks) Pro/Basic features beyond the website. It is difficult to differentiate the features as an entry level CNC'er. SprutCAM lists their features on this page:
http://www.sprutcam.com/Products/#Compare

It appears that most people will need the "expert version" $3000 US, and that the machinist version is really more of a previewer's tool?

Rhino CAM Pro $2000 US a.k.a. MillWorks features are listed here:
http://www.mecsoft.com/Mec/Products/products.shtml

Millworks has a good PowerPoint presentation that can be viewed from their website. Does SprutCAM have something similar I can review?

Jim

[dave@sprut.co.uk]

Hi Jim,

I cannot give you any comparisons regarding RhinoCAM because I have never seen or used it myself, sorry.
The main difference between the Machinist and Expert versions of SprutCAM are that the Machinist version does not apply cutter paths directly to a solid/surface model, whereas the Expert version can do. Other than this the two are identical.
Expert = 2 / 2.5D & 3D
Machinist = 2 / 2.5D
Both are 3 + 2 axis.
Postprocessors are included, and we can output native ShopBot code.

There is a downloadable Powerpoint Presentation for SprutCAM here:
http://www.sprutcam.com/Downloads (Presentation section).

I am working on some video tutorials which you may find useful here:
SprutCAM tutorials (http://www.sprut.co.uk/37402.html)
I am trying to add to these as time allows.

You are more than welcome to try either the full Machinist or Expert versions for 30 days. I am happy to give one to one online demonstrations, please e-mail me for download instructions or to arrange a convenient date/time for a demo.

Dave

[jim_staud]

Dave,

Thanks, looks fairly user friendly. Good presentation with the sample machine paths and task panels.

I will make a comparison between SprutCAM and MillWorks, and let you know my results.

Is the 30 day trial version the basic SprutCAM or the advanced? Can the trial version cut a sample geometery for proper comparison?

I would like to make a sample file of the level of detail that I expect to be able to use SprutCAM for and see if there are any issues that can't be resolved expeditiously.

Jim

[dave@sprut.co.uk]

Jim,

The 30 day trial can be either the Machinist or Expert version, just indicate your preference when applying for the activation code.
The trial version is fully functional and you can cut as many sample parts as you wish.
Let us know which postprocessor(s) you require and we will make this available and will be happy to undertake any modifications that may be required.

Dave