# Chatter & the Tormach



## echesak (Sep 3, 2014)

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


----------



## billdeme (Sep 3, 2014)

. 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.


----------



## echesak (Sep 3, 2014)

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


----------



## Cheeseking (Sep 3, 2014)

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


----------



## echesak (Sep 3, 2014)

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


----------



## billdeme (Sep 3, 2014)

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


----------



## ecdez (Sep 3, 2014)

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.


----------



## Ken_Shea (Sep 3, 2014)

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


----------



## echesak (Sep 3, 2014)

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


----------



## Ken_Shea (Sep 3, 2014)

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


----------



## echesak (Sep 4, 2014)

Well, no Video.  I'll probably be trying this one again tonight with a HSS 3/8" 3 flute EM.  If this looks OK, I'll shoot a video of this one.  It's coming around, and the suggestions here have been helpful. 

I also took a quick look at the feeds and speeds spreadsheet, but didn't really see how it worked.  Seems that the formulas in the answer spots are empty.  I'll look at this in more depth again.

Eric


----------



## Ken_Shea (Sep 6, 2014)

Eric,
Just in case you have not seen this guy on YouTube check him out.
He uses a Tormach and is pretty descriptive on what he is doing so it's easy to pick out the details of things that may be of interest to you.

I'm not sure if linking is permissible and I don't want to ruffle any feathers, just go to YouTube and search for NYC CNC.

Ken


----------



## echesak (Sep 6, 2014)

Thanks Ken.  Yes, I'm very familiar with this series.  I've been through the entire set a couple times.  Thanks for the reference, though...

I've made a ton of progress, over the last couple evenings.  I've tried some of my better bits in the Tormach with fantastic results.  The short stick-out really helps a lot.  I was trying a 3/8" International Minicut last night.  It rips through the aluminum at a really good rate.  I was conservatively cutting at about 0.100 DOC, 20IPM, 5000RPM and 40% step-over.  It was eating this up with no problem at all.  I probably could have doubled the feed.  The finish is not as good as I'd like.  But the Minicut bit is a rougher. 

I'm starting to get a feel for what seems to work.  I want to try my 4 flute finisher again, and see if it works better on some of these new settings, but for finishing, not hogging material.

Thanks to all for the tips and info.  I'm definitely making progress.

Eric


----------



## Ken_Shea (Sep 7, 2014)

That's good news Eric,
It takes time to learn ones equipment and for us Hobby guys that aren't at it day after day it takes a bunch longer. On of the things to look our for on smaller lower power machines like ours is at high RPM motor torque drops significantly and while the servo's can still push the table at max rate it can just bog down the motor if you get too aggressive.
Four flute on Aluminum works well as a finisher or on some of the tougher aluminum alloys for general non aggressive use.

When you get some cash ahead I'd sure invest in a good machining calculator, I use MEPro and HSMAdvisor both are very helpful and both seem to have their strong suit, also both developers are great guys and very attenative to input and any issues. HSMAdvisor has a online free version that is very useful for day to day use kust not all functions are fully implemented.

I machined two swivel components for the cyclick control on a helicopter I am building, got them done (to the first stage) and they turned out excellent but sure nothing I was proud of with regard to tool path efficiency, was terrible, I just got tired of trying to program the perfect tool-path and wanted to make my mill messy 

I'd been away from it for some time ai it showed.

Ken


----------



## echesak (Sep 7, 2014)

I've been looking at the different options for speeds and feeds, including the spreadsheet listed earlier in the thread.  I can see the value, I just didn't have much confidence in them.  But after my last run with the 3/8 rougher, I plugged-in my experimental numbers and found that they do indeed match the ones calculated.  I guess I just needed to prove that to myself.

Helicopter parts.  Humm, interesting.  I have had an interest in all man-made flying things, since I was a kid.  My oldest daughter is studying Aerospace Engineering.  I'd be very interested in seeing photos of what you're working on. 

Eric


----------



## Ken_Shea (Sep 7, 2014)

Since it's quicker then taking a picture here is a screen shot of the assembly, the part being machined now is the blue section. When I get that done I'll take a pic and show you installed (temp) on the frame.

Be sure and tell you're daughter that one requirement of an aerospace engineer is to offer free advice to those on HM, I don't think she will fall for it but it's worth a try.


----------



## echesak (Sep 7, 2014)

Ah, very interesting unit.   So what heli are you building?

I'm sure my daughter would have no problem offering advice to HSM'ers.  My other daughter is studying EE, so between the 3 of us, we should have most everything covered (ME, EE & Aero).

Thanks for sharing the screen shot.

Eric


----------



## Ken_Shea (Sep 7, 2014)

ME, EE, Aero, wow, I'd definitely be building something cool.

What I am doing is not professionally engineered but it is designed with a great deal of thought and research.

This Helicopter design is old, actually, I had built one around 1971. While basically the same design this build is refining lots of areas that were, well, just too home built for my taste, that is not to say they did not function as needed because they did and the design allowed for the kit builder not to be required to machine components.  It was called a Commuter II. It was the basis for the current manufacturer of the Safari Helicopter kit.

You have plans for building something, big or small now that you have you're Tormach?


Ken


----------



## DaveSohlstrom (Sep 8, 2014)

Ken

The helos look like mini bells. At 133k for the full kit it is out of my price range. Soloed a Hughs 300 back in 1980. Would rather fly rotor than fixed wing.

Dave


----------



## Ken_Shea (Sep 8, 2014)

DaveSohlstrom said:


> Ken
> 
> The helos look like mini bells. At 133k for the full kit it is out of my price range. Soloed a Hughs 300 back in 1980. Would rather fly rotor than fixed wing.
> 
> Dave



They are way out of my price range as well Dave, that's why I am building 
Helicopters are flat out fun, nothing can compare to the flight freedom in them.


----------



## CNC Dude (Sep 28, 2014)

Hi Eric,

Some input from a fellow Tormacheer. For Speed and Feeds I have been using GWizard. It is definitely not as economical as the Excel sheet you guys have been talking about, but there is a LOT of stuff in there! 

Bob Warfield, its creator, also has a lot of information on his website (CNC Cook Book) and that has helped quite considerably. Since I only use the machine every now and then, I have forgotten every single thing I ever learnt, but I do recall the information is quite valuable.

Now, this SW is a subscription based package (which really drives me nuts because I like buying the SW, not renting it!), but for Tormach owners, they have a lifetime version you can purchase at an economical price. And BTW, they throw specials every not and then and it is even more economical. Right now it is priced at $79, but I have seen it as low as $59. That may have been a one time deal, though.

I am not certain if you have already contacted Tormach, but if you give them your information (e.g. machine serial number), they will add you to the list and you will become a Tormach Owner which is how you can take advantage of some of their deals. If that interests you, of course.


----------

