-
I want to thank all the members that have upgraded your accounts. I truly appreciate your support of the site monetarily. Supporting the site keeps this site up and running as a lot of work daily goes on behind the scenes. Click to Support Signs101 ...
having problems routing 1/2" aluminum
- Thread starter Darren123
- Start date
SignosaurusRex
Active Member
Do you know what grade (Hardness) of aluminum you are using?
KR3signguy
New Member
Are you using a down spiral? Just a thought.
The Big Squeegee
Long Time Member
When the aluminum sticks to the cutter it will build up heat as well as become harder to move through the material. An oil or wax will help to keep the aluminum from sticking. You can also increase the chip size by slowing the speed of the cutter or increasing the feed speed.
The kind of material will also make a difference. 5051 is a soft aluminum. 2024 and 7075 are much harder. The softer the metal the more it will stick to the tool.
The kind of material will also make a difference. 5051 is a soft aluminum. 2024 and 7075 are much harder. The softer the metal the more it will stick to the tool.
J Hill Designs
New Member
I've had great success with 1/4" bit and a 4-pass to cut with the last one being cleanup as well - just my 2 cents
Westcoast Sign Guy
New Member
How many flutes? What make bit? What were your F/S's? What hold down method?
I have found Crisco to be very effective on difficult materials. In regards to grades, aove is correct. 5051 has the lowest copper content, and 7075 is the highest. The T number following the grade is the hardness, typically these grades are t6. Other factors change the machinability of aluminum, for example if its been welded, the hardness will have been annealed out of the material as soon as the aluminum has cycled above about 4-500 degrees. As to the worst I have had the pleasure to worked with, extruded shapes (3XXX series) takes the title. Even that has tricks to make cutting and tapping simple.
1/2" aluminum should NOT need 4 passes.. You can do it in 1 if you know what you're doing. I run a 1/4" spiral upcut bit @ 126IPM @ 28000RPM and it cuts just fine. Make sure your mist is working correctly and turn it up a little if needed. I don't adjust my mist too much. Make sure your parts aren't moving on the table (tabs or onion skin methods..).
Forgot to add.. Often times, going too shallow with cuts will break bits.. 4 passes @ .5" comes out to 1/8" per pass.. Too much material being cut by tip of bit will break it in minutes. Your tip will wear really fast and break. Typically, you want to go to a depth of the diameter of the bit: 1/4" = 1/4".. Decrease your speed by 25% per pass.. So, .5" is 2 passes on 1/4" bit.. can be done in 1 if speed is slowed by 25%.
Jester1167
Premium Subscriber
The width of the bit = the max depth of cut in aluminum. 1/4" bit = max 1/4" depth. With deep cuts orient your two mister nozzles so that a majority of the time they are blowing down into the tool path not just on the exposed bit.
Exactly. Don't have your mist nozzles directly opposite each other.. If the spindle were a clock face, one would be @ around 12:00 and the other @ 4:00. So, staggered. This way, you're getting fluid in all areas.