Need Help Help milling alupanel

[Mike Pickett]

Hello everyone, we have a Summa F1612 auto depth control. I am milling 2mm alupanel and the machine does a horrible job. We end up having to file every piece we cut. I am running at 16500 rpm at 30 mm/s with 2 equal depth cuts and no finishing pass (I have tried the finishing pass but it doesn't seem to change quality of the mill job). I am using a 52 series double flute upcut bit. I have also tried a 63 series single flute upcut bit. 2 things...the bits don't do a good job and they don't last long at all. I understand it could be the sacrifice mat but when I change it out often nothing changes.
What do you mill your alupanel at?
What kind of bit do you use?
What is the quality of the job like?

 

[Ian Stewart-Koster]

Are you 'milling' it, or just trying to cut the perimeter of a shape in it?

 

[Mike Pickett]

You can cut it alot faster with a stouter router but a good place to start is 18,700 RPM, 60ipm (which looks close to 30mm/s), 1/8" bit should manage a single pass without fluid. Try cranking up your RPM's, and perhaps changing to a different bit. Looks like the summa takes traditional bits, but I didn't see any info referring to the 52 series. In any case, Belin makes a fine routing bit, I recommend the 33317A for something like this, 1/8" diameter single flute upcut, runs about $20-25 from Reese supply in my area.

Thanks for the info!

 

[MoultrieMade]

My current formula for 3mm ACM is an Amana [HASHTAG]#51446[/HASHTAG] (1/8" O-flute) at 19,000rpm and 125ipm, conventional cut. I do one full-depth pass with a 0.005" offset, then a second pass with the same feed/speed but no offset. This gives me a good edge and ejects most of the chips that otherwise like to stick to the edges.

 

[signage]

why would anyone mill ACM?

 

[Mike Pickett]

Thanks for the info!

Are you 'milling' it, or just trying to cut the perimeter of a shape in it?

I am cutting out shapes in a piece of alupanel, with the router.

 

[Mike Pickett]

My current formula for 3mm ACM is an Amana [HASHTAG]#51446[/HASHTAG] (1/8" O-flute) at 19,000rpm and 125ipm, conventional cut. I do one full-depth pass with a 0.005" offset, then a second pass with the same feed/speed but no offset. This gives me a good edge and ejects most of the chips that otherwise like to stick to the edges.

Thank you, this is perfect! With the couple of suggestions I got I can play around with it a bit and try for a better cut.

 

[Mike Pickett]

why would anyone mill ACM?

Interesting reply, could you please extrapolate as to how you do it. That would be helpful.

 

[Flatbed Tools]

Hello everyone, we have a Summa F1612 auto depth control. I am milling 2mm alupanel and the machine does a horrible job. We end up having to file every piece we cut. I am running at 16500 rpm at 30 mm/s with 2 equal depth cuts and no finishing pass (I have tried the finishing pass but it doesn't seem to change quality of the mill job). I am using a 52 series double flute upcut bit. I have also tried a 63 series single flute upcut bit. 2 things...the bits don't do a good job and they don't last long at all. I understand it could be the sacrifice mat but when I change it out often nothing changes.
What do you mill your alupanel at?
What kind of bit do you use?
What is the quality of the job like?

Hey Mike.

Our Rs404 - (4mm cut diameter with a 6mm shank) Polished Single O flute - Up Cut with nACo coating is extremely popular and has been tested on these ACMs for the best Quality.
For a production environment you could run at 45,000 rpm with 8"/second (480"/min). Some feel like this is too fast so remember that chipload with RPM + speed/feed has a special formula. You can then run the following with similar outcomes:
15,000 rpm - 2"/second (120"/minute)
30,000 rpm - 4"/second (240"/minute).

All these can be one pass, but I often recommend a clean up pass (subjective).

Let me know if you need anything further.

 

[signage]

Milling is usually referring to removing of material from a surface. What you are talking about it cutting, most materials I cut are done with a shear, saw or router.

 

[rossmosh]

Hey Mike.

Our Rs404 - (4mm cut diameter with a 6mm shank) Polished Single O flute - Up Cut with nACo coating is extremely popular and has been tested on these ACMs for the best Quality.
For a production environment you could run at 45,000 rpm with 8"/second (480"/min). Some feel like this is too fast so remember that chipload with RPM + speed/feed has a special formula. You can then run the following with similar outcomes:
15,000 rpm - 2"/second (120"/minute)
30,000 rpm - 4"/second (240"/minute).

All these can be one pass, but I often recommend a clean up pass (subjective).

Let me know if you need anything further.

Please note, these are specs for a single flute cutter. If you cut with a 2 flute, you'd cut the RPMS significantly down. Approximately 1/2 the speed.

ACM cuts pretty easily but it does have an issue with the edges. This is down to cutters dulling quickly. You'll often notice a cutter works great for the first few cuts and then things get worse. Some of this is down to the quality of the cutter and some of it is down to premature wear due to wrong feeds/speeds. One other issue with ACM is the variability of the top layer both in thickness and type of material. Also, you're only using the same 1/8" part of the bit every time. On thicker materials, you're getting more bit engagement which can help too.

Big picture, I'd look into the cheapo carbide bits from eBay (Drillman1 is a well known seller). You can throw them out regularly and they're pretty decent quality all things considered. I like the 2 flute 1/8" bits more than the 1 flute 1/8" bits.

 

[Flatbed Tools]

Please note, these are specs for a single flute cutter. If you cut with a 2 flute, you'd cut the RPMS significantly down. Approximately 1/2 the speed.

ACM cuts pretty easily but it does have an issue with the edges. This is down to cutters dulling quickly. You'll often notice a cutter works great for the first few cuts and then things get worse. Some of this is down to the quality of the cutter and some of it is down to premature wear due to wrong feeds/speeds. One other issue with ACM is the variability of the top layer both in thickness and type of material. Also, you're only using the same 1/8" part of the bit every time. On thicker materials, you're getting more bit engagement which can help too.

Big picture, I'd look into the cheapo carbide bits from eBay (Drillman1 is a well known seller). You can throw them out regularly and they're pretty decent quality all things considered. I like the 2 flute 1/8" bits more than the 1 flute 1/8" bits.

To piggyback off this and the feed/speeds comment. Running slow has a dramatic effect on bits dulling. Aluminum is very soft and when routing slow, the aluminum has time to melt and severely dull ANY router bit or even stick to the router bit, which will kill it almost immediately. Also, the coating on certain bits prevents heating, which prevents dulling.

If you are currently running at "16500 rpm at 30 mm/s (1.8"/sec)", this is too slow. You should change to a single flute and run faster (settings I sent). We have done a case study where we routed 60 - 4x8 sheets of ACM (Dibond) on a single bit (Rs404). The cut file was 2' by 4' rectangles (6up/sheet). I know Dibond is cream of the crop, but maybe you have a similar job to do a different case study on Alupanel? Let me know!

 

[Mike Pickett]

To piggyback off this and the feed/speeds comment. Running slow has a dramatic effect on bits dulling. Aluminum is very soft and when routing slow, the aluminum has time to melt and severely dull ANY router bit or even stick to the router bit, which will kill it almost immediately. Also, the coating on certain bits prevents heating, which prevents dulling.

If you are currently running at "16500 rpm at 30 mm/s (1.8"/sec)", this is too slow. You should change to a single flute and run faster (settings I sent). We have done a case study where we routed 60 - 4x8 sheets of ACM (Dibond) on a single bit (Rs404). The cut file was 2' by 4' rectangles (6up/sheet). I know Dibond is cream of the crop, but maybe you have a similar job to do a different case study on Alupanel? Let me know!

This information is great! We are cutting something similar to license plates on a 4 x 8 sheets. We get 68 plates from a sheet. The problem is the bit does a poor job very quickly and we have to file the edges smooth on the plates, which triples the production time. I will normally get 3 sheets before we can't use the bit anymore, which has always felt off considering aluminum is so soft.

 

[SignEST]

Higher flute counts and CNC routers aren't friends unless you're cutting foam. The RPM is just too fast. At 16500 and 2 flutes you would need to go at 100mm/s minimum. Not sure if your vacuum can hold that down.

If you have an extra spoilboard out of MDF you could always use a downcut but then there's a bit of a mess to clean up from the table afterwards.

 

[klikn]

My current settings for a perfect edge:
Chinese 1/8" Single O flute - Up Cut
Pass depth: 1/8"
Spindle speed: 15000rpm
Feed rate: 1900mm/min
The direction of cut: Climb

 

[MJ-507]

I think his point is that milling is a somewhat different operation than routing, though plenty of people interchange the two terms since it is in essence milling, but somewhat inaccurate to call it that.

Milling is more than a somewhat different operation - it is a totally different operation. I've never heard anyone in my career (25+ years) refer to cutting shapes as milling. As long as I've been around, milling is removing material & cutting is, well, cutting out shapes. Maybe the terminology is a location thing but I've worked up & down the East coast & this is the first time I've heard of this.

 

[CanuckSigns]

We run our summa F1612 at 38mm/sec @ 25,000 RPM in a single pass and get great results, this is the bit we use: https://www.betterbits.ca/M-P_bit_selector

It sounds slow, but you need to remember the standard router on the summa is pretty much a glorified dremel, it can't handle the excess forces that a proper CNC router with a spindle can!

I had originally ordered some router bits from china @ $5 each, and the quality was hit or miss (shocking I know!) some bits worked great, others lasted a few cuts before they got too dull. since switching to these new bits I've had much better luck

 

[GaSouthpaw]

The confusion could have something to do with router bits being termed "end mills" by some manufacturers.
As for the speeds- with a .125" bit, I'd be going about 150 IPM @ 24K RPM, most likely in a single pass on 4mm ACM.

 

[Josh Martinez]

This material should cut pretty easy. We have lots of customers cut this material. I would recommend a 3/16 or 1/4" tool. We offer a coated tool that will last longer. Its a little more expensive but may work better for your application. You can use the single flute Viper XVO2232 run it at 19,000 RPM at 150 IPM conventional cut in a 1 pass. Or for longer tool life use the Viper Black XVO2232-DLC run it at 19,000 RPM at 160 IPM conventional cut in a 1 pass. I'll put link below. Hope this helps.

Viber Black Series (Aluminum, ACM, wood, etc.) Archives - X-Edge

The “Black Series” tools are DLC coated (diamond-like coating) to provide low friction dry cutting of aluminum. Viper Black DLC coated tools are corrosion resistant and have self lubricating properties which also allow them to be a longer lasting alternative to the standard Viper series tools.

www.xedgetools.com

Viper Single Flute Upspiral Archives - X-Edge

The Viper single flute upspiral is a great all-round tool that performs well on a wide range of materials from aluminum, ACM, wood, plastics, etc.

www.xedgetools.com

 

[Ian Stewart-Koster]

Pardon if I say it, but I find it odd reading that anyone has a problem with routing ACM.
We use standard 2-flute cheap chinese 1/8" upcut end mills, and have for the last 14 years.
Our router is ancient, so we nurture it a bit, but 35mm/sec at full depth, single-pass, I can't recall having a problem. Just adjust spindle rpm as required.

If the top edge is looking a bit rough, get a new cutter. If you buy a pack of 10 for $5 or so, they're not an ordeal to toss out. If your edges are looking poor, maybe you got a bad batch of cutters?

I've also got expensive Onsrud cutters for high quality work, but ACM is about the easiest you'll get.
I leave the swarth in place to help hold the parts - we do not have a vacuum bed, and I tek-screw the sheet corners down to the MDF bed to secure the substrate.