Help Require to Engrave Aluminum in a CNC Router

[hardiknsheth]

Dear All : I would thank you in advance for your responses.. I am using CNC Router for Woodworking and engraving relief on Wood and MDF since 2 years, without any trouble. Now, recently I purchased new Router to engrave in Aluminum, but after loosing several tools even in roughing process - I did not get any results.

My machine is having a following specification
4.5 KW Air Cooling Spindle
Max RPM 18000
Mist Cooling System
(Using Kerosene as a coolant)
2500x1300x300 mm working area.

The first design I started is attached and its 600 x 600 x 6 mm in Size.

Aluminum I am using is extruded grade 6061.

The tool and tool path, I tried for rouging is
Endmill 3mm and 3.175mm and tried
2, 3 and 4 flute tool.
9000 RPM and 18000 RPM
with 0.2, 0.25 and 0.3mm Deep cut
with a 1.5 to 3mm stepover
and 600 to 2000 mm/min feed rate,
in combination with above all.

But after a while the tool gets broken and the chips are melted inside the flutes of the tool.

I would request you to please suggest me what would be the right way of doing this design in aluminum in the above size.

[aarggh]

I'm sure other's will have more knowledgable answers coming but the potential problems that springs to my mind right now based on what I've done is:

1 - you have very narrow cutters machining a very large piece of aluminium.
2 - the feedrate is very substantial, especially given the size of the cutter
3 - the pass depth and stepovers I would halve, especially again as you are using a small cutter
4 - the spindle speed may be too fast, heating up the cutter
5 - are you clearing ALL the waste as it occurs?
6 - I generally get better results from 2 flute upcut spiral cutters as the endmills tend to clog straight away, at least for me anyway!

From my little amount of observations machining aluminium, a smaller cutter being forced through large material at substantial depth passes would be flexing, and heating up very, very dramatically. With 1/8" endmills in a 4.5kW spindle, I imagine it as akin to sticking a toothpick in the barrel of a jack hammer and using it to punch holes in mud.

Seeing as you have a 4.5kW spindle, buy some 2 or preferably 3 flute upcut spiral cutters suitable for aluminium in a much larger diameter, so they won't flex, will cut more material, faster and easier. At least for the roughing anyway. Maybe split your roughing passes into one at 0.5 clearance for the larger bit, then 0.35 clearance for the smaller roughing bit, then take shallow passes at a slower feed for the finishing cutter but not so slow it creates heat buildup.

These are my observations, and they work for me, but may not suit everyone.

cheers,
Ian

[hardiknsheth]

Hi Ian..

Thanks very much for your suggestion, I really appreciate this. I used a larger tool as you suggested and tried it on this job, and found out that the problem with the larger size cutter would be tiny areas - which are smaller than the diameter of the tool, so the ArtCam toolpath just ignores the smaller places and does the roughing tool path - this will create a bigger problem in at the time of Finishing, as the tiny areas has the more metal remaining and it will break the finishing tool, unless I do the finishing in slices, which will be a huge amount of time and won't be viable. I will try to find a better tool path generation software.

Thanks again for your suggestion

Cheeers !
Hardik

[aarggh]

Hi Hardik,

You most likely don't need new toolpath software, if you need to get fairly high detail, just generate multiple roughing passes as I mentioned previously, so the bulk of the material is taken off by the largest cutter.

For example, if you need to use a 1/8" cutter for high detail on the finish pass, and your allowing one or preferably at least two passes at around 0.3-0.4mm allowance, then create your first roughing pass using a larger cutter and set it to 0.6mm or 0.5mm, then create a second roughing pass using a 1/8" higher detail roughing cutter to a depth of 0.4mm. So all up you run the large cutter first, taking the bulk of the material off, then a second roughing pass taking a shallow pass, then finish with the high detail pass or passes. Takes longer, but this way you can actually run a higher feedrate as your taking shallow passes and not stressing or heating the bit too much.

Just pay attention to how it feels, and more importantly, how it sounds. One other thing I forgot to mention, on a sheet this big, it would be a huge advantage to not just clamp the sheet down, but also generously use double sided tape to ensure the sheet isn't vibrating under the cutting load. This aspect alone can make a huge difference, machining metal sheets that are clamped at the edges can sometimes be disastrous for cutting, usually it's making a racket if this is the case.

Another thing to look at, is the software your using generating the appropriate toolpath patter and direction to suit the bits your using? In other words, is it using conventional/climb-offset/raster pathing, etc?

Something else to make life much easier for you Hardik, buy some bits that are large shank but small cutting width, they are very, very cheap on Ebay, probably 6-12mm cutting length will do you fine, and being larger shank they will be far less prone to flexing and bending, so you can probably bump up the feedrate and the pass depth! You may even be able to go to smaller than 1/8" finishing with them, although obviously the cutting width would be directly proportional to the cutting length. The shorter the cutting length, the narrower the cutting bit you can, within reason anyway.

This link has some info you may find an interesting read:
http://www.haascnc.com/solutions_3D.asp#3D

cheers,
Ian