Vitesses de coupe et d'avance pour l'alu ?

[oric1]

Bonjour,

Je commence à maitriser la bete, mais je suis un peu perdu sur le reglage des vitesses d'avance et de rotation.
Ma principale utilisation est l'usinage de face avant 19" en alu , epaisseur max 4mm.
J'ai acheté des fraises, à 1, 2 et 3 dents pour l'alu en 3mm et 6mm, mais je ne sais pas comment les utiliser et quelle est leur durée de vie.

La finition de ma derniere facade n'est pas geniale. Les réglages ne doivent pas etre correct :

- Broche Kress 1050-1
- fraise 2 dents 3mm
- avance 200 mm/min ( 3.3 mm/sec )
- passe 5/10
- rotation 12000 tr/min

Merci de votre aide.

[ymasquel]

Bonjour "Oric1",

Bien qu'il y ait d'excellents praticiens de la CNC et surtout des utilisateurs de la "profiler" parfaitement capables de te renseigner sur ce forum je crois qu'il serait utile de voir ce que disent les fora plus spécifiques à ces machines ainsi que quelques sites dont la page pratique de CNC LOISIRS est un bon exemple.

Amicalement, Yves.'

[oric1]

Bonjour Yves,

J'avais déja vu ce site, mais je n'avais pas trouvé grand chose pour l'alu.

@+

[boeingbrown]

Hi ?? (Oric1),

Apolegize for the other linguage.....
Writing this en Francauis will cost me a day and a worn dictionary ...

If you do a Google search on : milling aluminum speeds you will find several usefull references e.g.:

http://www.moldmakingtechnology.com/articles/030702.html

BUT, but:

Most numbers have been achieved in ideal situations, with big stable machines etc.

Since the Profiler is a small machine it is not capable to absorb too much vibrations which are generated during higher forces.
This means that in general is advised to reduce the advised numbers by 50 %.

Even after thsi correction you have to find YOURSELF what in your situation, with your machine, with your table it stands on, with your type of aluminium (harder mills better than soft !), with your type of end mill (none or a more special tip for biting in aluminium) gives good results.

So e.g. start with 3 mm flat end mill, good good good fixation of the material, 2 mm /sec and 0.1 mm per layer.

Although wrong for aluminium(!), start with Kress stage 3-4 (so 20000) rpm. This has the least risk of unwished vibrations. Can give more heat, so cool with lamp oil. later on reduce rpm if possible (but staying at this rpm is no problem and you will see that even cooling is not necessary; mill hand warm).

Take form this Dutch Profiler forum this thead and pick the links.

http://www.elektor.nl/forum/forum/actuele-projecten/profiler/aluminium-tips.1010276.lynkx?highlight=jure

And read what Jurai from Colinbus wrote, hes an expert (I'm not).

To all,

To start with there is aluminum you can mill and aluminum that it's harder to mill.

Aluminum that is in my experience the best to mill is AlMgSi 1 - 6082 or as in most of the dutch books "hard". Zacht alu is much more difficult to mill. This is because in the "soft" there is more aluminum.

One problem is cooling, other is speed.

First rule of the game is, never go deeper than half of diameter of the tool into the material. This is really important for the people that have weaker motors. By going deeper, the motor doesn't have the power to keep the RPM steady, and the RPM falls down which results in inappropriate feed for milling.

Second, if you started to slow and there is no adequate cooling (especially in soft alu) the aluminum sticks to the cutting edges of the tool. From this moment on, any tests you do will be wrong because the tool is not cutting any more!

Third, tool choice. Cutting lips. the less cutting edges you have the less problems you are likely to have. Less cutting edges means the tool is less in contact with material, meaning it generates less friction and therefore less heat. However, tools with more lips will provide better finish result but without cooling you won't do much.

From my experience, people say this. Let's mill alu. This is hard material I'll go slow. Let's try 5 mm/s. you start it doesn't work, then you don't change your tool and you start with cooling. And your speed is 3 mm/s. this then works a bit and then stops and at the end you mill at about 1 mm/s.

I usually mill alu in the following way.

For 1 mm tool 1 lip @ 24000 RPM 0.2-0.5 mm downstep 5 mm/s
For 1 mm tool 2 lips @ 24000 RPM 0.2-0.5 mm downstep 10 mm/s

For 2 mm tool 1 lip @ 24000 RPM 0.2-0.5 mm downstep 8 mm/s
For 2 mm tool 2 lips @ 24000 RPM 0.2-0.5 mm downstep 16 mm/s

For 3 mm tool 1 lip @ 24000 RPM 0.5-1 mm downstep 12 mm/s
For 3 mm tool 2 lips @ 24000 RPM 0.5-1 mm downstep 24 mm/s

However you must cool the tool. This I do either with own cool system or with methanol. But do note that just one spray every now and then is not enough. Don't save it it costs 2€ per liter and your tools much more. Don't be afraid to spray some on.

One more remark. In overall milling jobs, material has to be properly fixed. If you don't fix it good it starts to vibrate. This causes tools to break.

With 6 mm tools I mill regularly (i always use the biggest possible tool, but the motor is only 1 KW so I limit this to 6 mm). Speed there is @ 24000 RPM with feed of 60 mm/s 1 mm down.

You should generally mill less deep but faster. The most common fault for melting material is that the tool is too slow. If you start a job and you see that it starts to melt, lower the RPM of your motor. When the process is good, see @ what RPM you were and then recalculate your feed. Per example. You were milling something that was melting @ 24000 RPM and @ 5 mm/s. By lowering the RPM you come to conclusion that you have good result @ 12000RPM. This means you can mill the same part at the same result @ 24000RPM and 10 mm/s. If this was a single lip tool and now you are using a double lip tool then put your speed to 20 mm/s.
Hope this helps.
jure

Hope this helps too,

Hessel Oosten (Dutch Profiler miller).'

[boeingbrown]

And a short movie:

Attached below.

H.

[oric1]

Thank you "BoeingBrown",

I read it all at once....

Best regards.