Good day all, we received a new Tormach about 4 or 5 weeks ago. The machine is being used for injection mold work, mostly cutting 4140 and p-20 (prehard 29-36RC).

Machine limitations are becoming very apparent, torque is a problem. Low range doesn't have enough of it and high range has very little. Roughing pockets with cobalt roughers is problematic, using carbide to rough is nearly impossible.

I understand that it is a light duty machine, but it could be modified to be more powerful. A high torque motor would make a difference. There would be a lot more torque in low range, high range would also be a big improvement.

One other issue is the feed rates; do you think a servo conversion would be a big problem? Tormach offers consulting on this but they don't do it for cheap. Has any one of you switched to servo motors? If the feed rates could increase to at least 100 IPM, it would be a great improvement.

What other problems would the servos, or higher feed rates cause with the bearings?

Any input would be appreciated. These are just preliminary ideas and may not be worthwhile to pursue. If it can improve the machine then why not?

You gotta use smaller cutters (carbide is ok), go slower, and make more passes with less stepover.

Also, use a light mist cutting fluid with lots of air. (i.e. not flood)

It's not how fast you can remove material but how accurate. :)
A lot of patience will be your best solution.

HTH, Pres
Or, for around $100k a new HAAS can help you out.

I am using smaller cutters and going slow, it is cutting surprisingly accurate.

I am still working on the patience thing, it just hurts to know that it could be done in one hour and takes 4 or 5.


Or, for around $100k a new HAAS can help you out.

That is the next step were working on, the Tormach will then be for plastic or little jobs.

I think removal rate is not directly about torque it's about usable horsepower at the cutter. Keeping the rpm high (at least so the motor is running at its rated rpm) by selecting an appropriate size cutter will help keep the HP up and hence the potential removal rate.

Just curious, why are you keen for 100 ipm for mold making. I would have assumed you spend 95% of the running time cutting material at low ipm.

Regards
Phil

Good day all, we received a new Tormach about 4 or 5 weeks ago. The machine is being used for injection mold work, mostly cutting 4140 and p-20 (prehard 29-36RC).

Machine limitations are becoming very apparent, torque is a problem. Low range doesn't have enough of it and high range has very little. Roughing pockets with cobalt roughers is problematic, using carbide to rough is nearly impossible.

I understand that it is a light duty machine, but it could be modified to be more powerful. A high torque motor would make a difference. There would be a lot more torque in low range, high range would also be a big improvement.

One other issue is the feed rates; do you think a servo conversion would be a big problem? Tormach offers consulting on this but they don't do it for cheap. Has any one of you switched to servo motors? If the feed rates could increase to at least 100 IPM, it would be a great improvement.

What other problems would the servos, or higher feed rates cause with the bearings?

Any input would be appreciated. These are just preliminary ideas and may not be worthwhile to pursue. If it can improve the machine then why not?

Just curious, why are you keen for 100 ipm for mold making. I would have assumed you spend 95% of the running time cutting material at low ipm.

Regards
Phil

Im actually looking for 500+ IPM, for 3-D surface finishing of cavities. (not from the Tormach though, I am not that crazy) From the Tormach I would like to try and get 100IPM.


As far as appropriate cutter size, I find it to be a pain using only a 3/8" to pocket out a fairly large cavity.

Im actually looking for 500+ IPM, for 3-D surface finishing of cavities.

Maybe want to be looking a machines with names like Yasda and Roders then.


As far as appropriate cutter size, I find it to be a pain using only a 3/8" to pocket out a fairly large cavity.

Bigger cutters need more HP, without enough power metal removal rate drops as the cutter gets larger.
More HP requires a larger machine or you will beat the slides and screws to death.

Maybe want to be looking a machines with names like Yasda and Roders then.



Bigger cutters need more HP, without enough power metal removal rate drops as the cutter gets larger.
More HP requires a larger machine or you will beat the slides and screws to death.


I realize that its impossible to get to that feed, but 100IPM should be more than possible.

Big cutters need more HP, I understand that but a 1/2" endmill is not that huge.



Wow with all the responses so far, this is almost starting to seem like a bad idea......................almost.

[QUOTE=Chuck Reamer;344741]Im actually looking for 500+ IPM, for 3-D surface finishing of cavities.QUOTE]

You have purchased the wrong machine if you want 500IPM. Don't get me wrong, the Tormach is a great machine for what is was designed for. It was never designed for 500IPM. You will need to spend allot more money to get those speeds.

Willy

You have purchased the wrong machine if you want 500IPM. Don't get me wrong, the Tormach is a great machine for what is was designed for. It was never designed for 500IPM. You will need to spend allot more money to get those speeds.

Willy

I don't want or expect 500IPM from the Tormach, I was just responding to philbur. He was wondering why I would want 100IPM for mold work.

I agree the Tormach is a great little machine, and is even more than expected. With a little extra modification it would be a lot better, I am just wondering if any one has done the same.

Hi Chuck

I would think that 100IPM would be easy for the Tormach. One of the main reasons for keeping it at 65IPM is it's open structure?

Willy

Hi Chuck Reamer,

I'm interested in the process for surface finishing. Could you please expand on this.

Regards
Phil

Im actually looking for 500+ IPM, for 3-D surface finishing of cavities. (not from the Tormach though, I am not that crazy) From the Tormach I would like to try and get 100IPM.


As far as appropriate cutter size, I find it to be a pain using only a 3/8" to pocket out a fairly large cavity.

I realize that its impossible to get to that feed, but 100IPM should be more than possible.

Big cutters need more HP, I understand that but a 1/2" end mill is not that huge.


No a 1/2" end mill is not that big and can be an advantage in softer stuff.

They tend to have the same number of cutting edges but can only be run at 75% of the RPM of a 3/8 for any given SFM.
In harder materials you often can not increase step over and feed enough to compensate for that without reducing tool life below that of the 3/8 tool. Because the larger radius of the tool means that for any given step over the cutting edge is in the cut longer and getting hotter and so it swings thru a larger temperature range every revolution.
And 1/2 end mills are 130 to 160 percent more money.



Wow with all the responses so far, this is almost starting to seem like a bad idea......................almost.

Not so much a bad idea as it is not a simple as it may seem.
I have seen a lot of hobby level machines that could feed at 100 IPM but very few that could accurately follow a complex tool path at that speed.


Personally I would go to servos just to get away from the singing stepper motors, I am not talking a servo motor with a step/dir driver either.


Philbur
Here is a good over view of this type of machining.
http://www.haascnc.com/solutions_3D.asp

Thanks for the link Andre but it still doesn't make it any clearer how you use 500 ipm to achieve a good surface finish. Even on a Tromach using 100 ipm at4500 rpm on a steel workpiece/mold is skating . What am I missing.

Phil

Philbur
Here is a good over view of this type of machining.
http://www.haascnc.com/solutions_3D.asp

Big mold with fine details requires a small ball end mill and small step overs on the finish passes. The tool path can get very very long.

You need the small step overs to get the finish, you need the speed to get done before you retire.
I have seen ball endmills 0.005" diameter being used with 0.0002" step overs

Big mold with fine details requires a small ball end mill and small step overs on the finish passes. The tool path can get very very long.

You need the small step overs to get the finish, you need the speed to get done before you retire.
I have seen ball endmills 0.005" diameter being used with 0.0002" step overs


I mill molds and always use the largest size ball mill possible to reduce the scallop height. The smaller the radius, the smaller the step over for the same finish (before I retire). In a big mold with details that allow, a 1/2" ball endmill is small.

Hi Chuck R - I have just got my PCNC and do mouldmaking also. I am encouraged by your thread. You talk about wanting more power and speed - but no mention off lack of ridgidity! That is good news for me!! Been doing mould cavities sometimes in P20 steel on my other little NC and ridgidity is the no1 problem. Vibration kills the cutters......So glad that is behind me.

Yes but not running at 4500 rpm and 100 ipm surely. It seems to me you would need xx,000 rpm +.

Lets say I have a 3 fluted 1/16" ball endmill and a maximum available spindle speed of 4500 rpm. What is a typical speed, feed, DOC and stepover for finishing a 3D surface.

What rpm and feed do you run your 0.005" ballend mills.

Phil

Big mold with fine details requires a small ball end mill and small step overs on the finish passes. The tool path can get very very long.

You need the small step overs to get the finish, you need the speed to get done before you retire.
I have seen ball endmills 0.005" diameter being used with 0.0002" step overs

Hi Chuck R - I have just got my PCNC and do mouldmaking also. I am encouraged by your thread. You talk about wanting more power and speed - but no mention off lack of rigidity! That is good news for me!! Been doing mould cavities sometimes in P20 steel on my other little NC and ridgidity is the no1 problem. Vibration kills the cutters......So glad that is behind me.

Rigidity is not to bad at all, a lot better than I expected. It is there, but I find it to be a lot better than the Bridgeport copy we had converted to CNC. I think you will be pleasantly surprised with it.



WOW a lot of talk about high feeds and speeds, for this machine the RPM would be the limiting factor with 100IPM. Rapid speeds would be so much quicker it would cut programs times by probably 10-15 percent. On a 7 hour program that makes a pretty big difference.

I read an article about a Millstar cutter that would rough at .013DOC and 300IPM in tool steel. Its all about the special cutters when high speed machining, light cuts and really high feeds.

I know any serious milling is just a pipe dream with this mill, but its still nice to get a little closer to that dream. At least for now, until a big new mill comes rolling on into the shop.

Originally posted by Philbur

Here is a good over view of this type of machining.
http://www.haascnc.com/solutions_3D.asp


That is a great link, I posted it in a Mastercam thread a little while back. Its a great link for anyone who is doing surfacing, it helped me with quite a bit of stuff. I still am having trouble with the filtering though, if anyone has any info on that.

What rpm and feed do you run your 0.005" ballend mills.

Phil

I have seen tools that small being used, I have never had the misfortune of having to use them.
A 100 SFM on a 0.005" dia. is something around 75,000 RPM so you end up being limited by the machine.

... I have never had the misfortune of having to use them.

:D

I can't comment on upgrading the stepper motors but something I have been hoping to do is upgrade the spindle motor. We cut allot of aluminum with 0.125 end mills and out biggest limiting factor is always rpm. I haven't had time to try and source a new spindle motor though.

levelzero,

Have you looked at the Sherline headstock as an auxiliary spindle? They sell an optional pulley to increase the speed to around 10,000 rpm.

http://www.sherline.com/4335pg.htm

Mike

you will not be able to 3D surface cut at high IPM with out exspensive conrtol
with look ahead capablilities,which the tormach does not have,even my hass cant do it,unless i pay 2,200 dollars for the look ahead option upgrade to the control,personally i think your asking to much from the tormach,it is the top of the line bench top,but its still a bench top,few months ago i bought a full size maching center at auction for $3,500,16 tool atc 600 imp,mayeb you should have looked around more

to at least answer one of your questions
yes,servo motors would be a great improvement,steppers have no power at high speeds where as servo make max power at top speeds and can accelerate faster and smoother,im not sure about what control tormach uses
but gecko sells a motion controller for steppers that improve smoothness and performance,and i think has some analog capablilities,i think its called t rex 100 or something,but check out what your control has ,maybe tromach has its own moition card,if not it would improve performance and is alot cheaper than servos and new drivers

i bought a full size maching center at auction for $3,500,16 tool atc 600 imp,mayeb you should have looked around more

I did look at a lot of used machines, unless I wanted a 18 or 20 year old machine, this was the best deal for the cash on hand. I am happy with it but that is still no reason to try and squeeze a little extra from it.

A old used mill can have all sorts of problems with it and can cost you a lot more than the purchase price in repairs. Down time is another major concern, with only one mill it could cause a major $hit storm for a machine to be down for a couple weeks

i agree with you there,i have other machines to pick up the slack if my old one craps out for awhile,im not knocking the tormach,last year i converted an x2 for fun,i ended up making around 4500 using and than selling it for what i had into it,i cut on 4 cavity mold on it,all 3d sufacing,came out great,but was real slow cutting,biggest cutter was 3/8 and smallest 1/8 ball
have you looked into carbide indexable tooling for your maching,you can rough alot faster and not dog the spindle,just a thought

have you looked into carbide indexable tooling for your maching,you can rough alot faster and not dog the spindle,just a thought

The only indexable tooling I have so far is a FAK engraving, spotting, chamfer tool from Ingersoll. I just recived a K-tools Octa mill, its a 1.25" high positive face mill. The videos on the Tormach site show a 1.5" Octa mill working well, my hopes are high and I will try it out some time soon.

I am not sure if getting a smaller indexable end mill will help the situation at all. My tooling suppliers recommend just sticking with solid carbide end mills. Is there any thing you could recommend for 1/2" or under indexable cutters?

I really like variable helix endmills the greatly cutdown on vibration and rough very well. I used to use a TiAlN coated HSS 3/8 rougher but the Vari helix roughs faster and lasts longer. I mostly use a 3/8 as they seem to last longer and have less cutting force. The one I'm using now just wont give up, its pretty dull and I push it a little harder every day, today roughing a lot of pre-hardened 4140, 1400 rpm, 5 Ipm, .300 deep .250 stepover. Oh and I use them in an ez trak. but they also get used in the vmc's where they run 7k
30Ipm with similar cut depth.

May work well in the Tormach.

Chuck Reamer, sounds like what you where wanting was one of these. LOL

http://www.ajaxcnc.com/cnc_mill.htm

There's a pretty good diff in money though, but the rapids are there. Although the spindle speed is not. 425ipm rapids & 375ipm cutting with look ahead though sounds just up your alley.


Jess