Chatter & the Tormach

echesak

echesak

Active User
Registered
Joined
Feb 17, 2014
Messages
97
Ok, so I'm making a little progress getting used to my Tormach (mainly the CAM software, Sprutcam). But I was looking for some feedback on tool chatter. I don't have a huge inventory of tool bits and was wondering what others use on their home CNC machines (Tormach and the like). Before I purchase any new end mills, I was hoping for some feedback. If you happen to know feeds and speeds, with particular tools, this would also be a helpful starting point.

Thanks,

Eric
 
. What is it that your exactly having an issue with? Keep things as short and stout as possible, the rest is feeds and speeds....... for the most part.
 
I'm new to CNC, not to general machining. I was working on my first metal (6061) CNC part last night and was getting a lot of chatter, throughout the program. I tried different feeds and speeds until I found something that was a little better. Generally, I was just looking for recommendations from others with a machine of similar rigidity, as to what kind of feeds, speeds, step-over and tooling.

Eric
 
What billdeme said. Can you tell us the cutting conditions - cutter type, diameter, is it carbide, hss - size, #flutes etc? What feed rate and rpms are you at? Depth of cut? Face milling? Climb cutting? Are the gibs adjusted properly? Coolant? Could keep going but in order to drill down to the problem maybe fill
in some more blanks and the picture will become more clear. Very jealous btw! Congrats on your new machine!


Sent from my iPhone using Tapatalk
 
Yea, sorry about that...


I was using an SGS 39147 3/8 dia, 4 fl, carbide coated EM. Here's the specs on that EM:

Milling - 3/8 X 3/8 SH CC 4 FL SGS TIN SOL/CBDE SEM, Square End Mills; Mill Diameter (mm): 9.53; Mill Diameter (Inch): 3/8; Mill Diameter (Decimal Inch): 0.3750; Number of Flutes: 4; Material: Solid Carbide; Length of Cut (mm): 25.40

I was milling 6061, climb milling, with a 0.09" depth of cut. Feed rate started at 10ipm, but probably ended-up around 5 or 6. RPM varied from 3000-5000, trying to squelch the music.

I'm reasonably capable with manual machining, but wanted to learn more about controlling chatter on the CNC. First off, I may have had the step-over set a little to high, but will need to get back into the program to see. The previous user of this machine, recommended 3fl, high helix carbide EM's at 2500RPM, but at a fed of about 20IPM and a step-over of about 5%. He gave me one of his end mills, so I'm going to re-do the program for a 1/2" EM and try this, hopefully tonight.

I really need to get some sort of enclosure built :)

Learning CNC has been interesting. CAM is a lot more complicated that I expected.

thanks for the assistance,

Eric
 
You should find that machining with cnc will give you a more controllable finish over manual. As im sure you know, NORMALLY higher feeds and slower rpms will quiet the ummmmm, music. I work with a lot of overhang, on a lathe, and ive found the opposite rings true.


MACHINING FORMULAS.SFM.= 0.262 x D x RPM
RPM.= (3.82 x SFM) / D
IPR.= IPM / RPM or CHIP LOAD x F
IPM.= RPM. x IPR
CHIP LOAD.= IPM / (RPM x F) or IPR / F
 
I found an excel file on another site that is pretty easy to use and gets me by for most of my stuff.



Not allowed to link to the site so this is the next best way. Copy and paste the below into google.


Speed And Feeds Combined Excel Calculators v27


First link that comes up should be for the "PM" site. Second post in that link has the file and it's free.
 
Eric,
Your feeds, speeds are quite conservative, nothing really wrong with the .090DOC but light machines are probably better off to decrease the DOC and increase feed to maintain a chip load
You will find with carbide end mills they will handle about all the RPM you have, they like RPM.
Maybe for aluminum a 3flute Aluminum cutting end mill would be better for chip handling.
A picture of your set up as mentioned earlier would help, also mentioned was the tool over hang, it needs to be as short coupled as possible the material also needs to be clamped well, if you are only biting a thin section it can cause lots of noise, in these cases feeds need to be slowed down.
Is it a new end mill?
I've no Tormach experience but have run a similar EM at 6000rpm, .125 doc and 50ipm in aluminum, on heavier mill but still not a large or ultra expensive one. Haas TM-1.

Ken
 
Hey... Great replies.

Thanks for the info on the S&F excel. Thanks also for the formulas. That suites me well.

...had a question for Ken_Shea:

What kind of overlap are you doing with that endmill and machine? BTW, I almost bought a TM1 when I was looking. My budget was a little short, but mainly the rigging and drywall work to get it into my garage is what changed my mind.


I just ran another set-up this evening. This time with a 1/2" 3FL Carbide EM. Stick out was pretty long, 2-3/8" . My DOC is actually 0.100". I was running a 40% Step-out (40% of the tool diameter), 3000 RPM and 15 IPM. The worked much better, with regards to surface finish, and chatter.

I guess I need to get used to feeding the bits what they want to take. I was always a very conservative manual "machinist". So these are aggressive cuts, in my book. I'd prefer longer cycle times over tool life. But I also understand that Carbide prefers heavier vs. lighter cuts.

Still plugging away at this. I took a video, I'll try to get it posted tomorrow, if my internet stays up long enough.

Eric
 
Eric,
I forget exactly but generally unless the tool path type requires something special hardley ever under 50% and often more. With that shallow a cut one could get pretty aggressive using carbide.
You could jump that 3000rpm up a bunch, not sure what the limit is on the Tormach.
I started on manual machines as well and had to fight with myself constantly to push the machine and cutters, still haven't gotten over it completely.
Was machining steel today, 1/2" 4fl Carbide, .050DOC and 30IPM with a 40% step over, could have easily gone faster but I don't like the noise and the material did not have a lot to grip on. which was part of the noise problem.

Ken
 
You must log in or register to reply here.
Back
Top