-
Aluminium sheet routing problems
Hi All,
I am hoping someone maybe able to help with our little problem.
Around 8 months ago we decided to expand into the metal fabrication field. All has been going well until now!
For some reason we seem to have developed a fault when routing the 3mm aluminium sheets on our Gerber CNC router.
The problem occurs when cutting out the tighter radius’s of letters in the aluminium sheet. The aluminium seems to be melting to the cutter causing the tool to rip its way through the sheet. Straight lines don’t seem to be a problem.
We have had our much trusted router engineer in who has checked the spindle and replaced the collet. He has now given the router a full bill of health and in his professional opinion it’s not a fault with the router.
The aluminium we have been using over the past 8 months has been 1050 half hard which our suppliers say is an industry standard? We have also tried using a harder aluminium 5251 half hard. The problem still occurs.
The speed and feed rates have not changed from when we first started routing aluminium.
Does anyone have any thoughts or solutions that may help?Dave
-
10 Replies
-
I believe this is being caused by the ambient temperature being higher than it was in the winter. Previously the aluminium didn’t melt because the heat generated by the cutting tool under those conditions was below the tipping point whereby aluminium would begin to melt. Now that it is summer, the current conditions mean it has moved beyond the tipping point resulting in the melting you are currently experiencing. (wait another 5 months and the problem will go away only to return again next summer).
Try speeding up the feed rate slightly in the summer months.
-
Many thanks Phil. I will give this a go tomorrow when our new cutters arrive and let you know.
Dave
-
As Phill says, but you might also try multiple (depth) passes along with increased feed rate, if you’re not already doing that.
-
New tools will probably help, do you have a flood cooling system or are you cutting dry? If dry then an air hose rigged up to a compressor will help remove heat. Try increasing the feedrate as has been said & don’t try to take to small a cut, slowing the feedrate or taking a very small cut will actually increase the heat generated as the heat should be removed with the chips.
-
The only thing I can add to what has already been said is to check the acceleration numbers. The tool slows down for the corners and then speeds up on the straight to prevent shakes.
This is user controlled on my router and probably yours as well.
Perhaps it is slowing down too much for the type of ally you are cutting.
My CNC has reset itself to default for no particular reason in the past…who knows why. Power surge, electrical storm, temperature change.Simon.
-
I now I’m a couple of weeks late in replying….
Wot the others said are all possible causes. I would like to add 1 more possible cause. If you are cutting in 2 passes, it can also result in the router bit clogging, especially with multi fluted bits. If you can, cut in 1 pass, and keep the feedrates up. Good chip loads actually cause the heat to be carried away in the chips you are cutting.
My choice for routing Ally (and composite, and Perspex ) is a 6mm single flute upcut bit. Use good quality (like Benlin) I cut at 30mm per sec (1800mm per minute) at 16 000 rpm. Ally up to 3mm is cut in 1 pass, 4,5 and 6mm is cut in 2 passes. With the thicker alu the heat still dissipates sufficiently.
Use a mister! If not fitted to your router, Q20 or the likes can also be used. Just expensive for volume work!
-
Hi dave first thing you need is some good tooling and a mist coolant system there is very few grades of aluminium which you can dry cut so a mist coolant system is essential you can buy them online for about £50 this will be the best spent money you will apply to any router take my word on this 16 years Cnc routing does not lie , next is your tooling and workpiece hold down I normally use 2 different tools both 6mm dia
One for a rough cut and a different one for he final cut I can get a mirror finish on my aluminium parts so believe me this works , I use a 6mm singe flute upward spiral cutter from itc with as much clearance in the tool this helps stop heat build up and prevents the aluminium moulding into the cutter surface but you need the mist coolant to help it once you hint the sweet spot on the cutter you should hear it change tone thats how i know if its machining well thats the must important part speed feeds and spindle rpm are not that critical run the spindle as hard as it goes 18000 or24000 rpm
What ever she does do your rough pass but do not cut right though and leave a .5mm to trim of on the final cut . Do your rough cut then change tool to a new one and do final cut with it feed rate about 40-50mm per second is what I normally run at but this normally depends on the aluminium . If this is a bit confusing give m a call on Monday and I an go though it better over the phone I cut aluminium all the time been machining it for 20 years so know a bit about it
Hope this helps dave
Moderator Edited to
conform with Board Rules
Please take a moment to read our Board Rules -
David, have to disagree with what you said about speed & feed rates, I would say they are very important, you will probably find that you have been doing it that long you just instinctively know how to set the job up correctly but the truth is you have pretty much hit the correct figures without thinking about it due to the experience you have.
-
Hi Martin speeds and feeds Are not the most important thing they are dependent on the material in general they will be somewhere in the region of 25mm per second up to 80mm per second you just need to give the cutter the chance to clear the chips away form the work piece cutting fluid makes a big difference to speeds you can run at also reducing vibration in the work piece is very important as well as cutting flute length all have factors I how fast you can cut alu.
-
I was cutting some 3mm brushed alu letters yesterday.
Since it was a mix of large and small letters, and me being a lazy sod, I decided to cut all at a slower (25mm per sec) federate at 12000 rpm.
Load the sheet, and run the program. I just hang around for a minute or so, adjusting the mist nozzles etc, and then go outside for a smoke.
Now, the first part of the program was hog cutting the insides of the letters, then the male cuts followed…….
When I come back after my smoke, I hear the machine sounding "different" while cutting. It turns out that I accidentally entered 250mm per sec, not 25! Fortunately, the specific tool – 6mm single flute – was set to a max federate of 100mm per sec. (With the Tekcel Enduro with ATC you can define max rpm, federate, acceleration etc for each tool)
Still, cutting 100mm per sec on just 12k rpm is seriously hauling arse! Maybe with a less powerful spindle (It runs a 9kW HSD spindle) or a less rigid gantry there would have been problems. Today I experimented with cutting at 16k rpm, and 50mm per sec, and it worked a treat. No chatter, and shiny, smooth cuts.
Log in to reply.