tormach 770 cutting 1018

[ccski]

Hello all, newbie here just starting out with cnc.
I have had my 770 for a few months and today was cutting a L00 lathe chuck wrench from 1/4 1018 CR plate.

Using G Wizard I set up 3/8 4 flute carbide at 3100 RPM (300SFM), 0.080 DOC, full slot 0.375 WOC, 15 IPM, 0.0047 IPR.
Cut started ok then stalled spindle several inches into the cut, I lowered DOC to 0.06 and feed to 10 IPM and completed the job after re indexing XY ( apparently the servo drive belt had slipped).

Question is... G wizard claims 0.3 HP so I thought I was safe at these settings, yet I stalled the spindle.
After completing the cut I examined the cutter under 10x and sad to say this brand new end mill looks worse for the wear.

Is there something I am missing in my calcs?
Any help greatly appreciated.

Similar Threads:

• Will cutting G10/FR4 fiberglass sheet cause a Tormach to rust?
• Internal Spline Cutting w/ Tormach possible (wheel hub)?
• Help with 1018
• Test cutting with Tormach 17mm insert end mill
• Tormach 1100 cutting wood

[RussMachine]

I'm learning not to be too aggressive with my 770.
I ran "big" CNC mills for years before getting my own 770, so my original programs were based on high speeds & feeds (As I was used to doing).
Boy was I wrong!
You have to slow things down, and kind of 'baby' the 770.
There simply isn't the same amount of rigidity and torque.
Be patient, you'll find that sweet spot often by reducing the feed and rpm a bit.
Also, try taking light cuts and more passes in 1018.
You'll get it done. TORMACH's can make any part a 'big' mill can, it just takes a little longer with lighter cuts and feeds.
For your 3/8 endmill, I'd try 2000 RPM, .030 DOC, and .003 IPR.

[lens42]

............( apparently the servo drive belt had slipped).........

Any help greatly appreciated.

Just to set the record straight. The 770 does not have servos. What happened is your stepper motor lost some steps when things bogged down.



Sent from my iPhone using Tapatalk

[kstrauss]

You mentioned running at 3100 rpm. Were your belts set for low range or high range spindle speed? You can run at 3100 rpm in high range but you have less than maximum torque available. It is a pain to move the belt but to get significant torque below 3500 rpm or so you must be in low. At 2500 rpm in high my 770 has trouble with even an aggressively fed 1/4-inch drill bit.

[MetalShavings]

I make very small parts using 1018 steel periodically and I've found through trial and error that the feeds and speeds recipes that my HSMA software churns out have to be reduced by at least a third the calculated values. In most cases I'll back off a little more than that. I used to use the G-Wizard generated feeds and speeds before I started using HSM and with those feeds and speeds too, I had to back way down on. Plus, with the G-Wizard F/S's I was just using the bottom face of my end mills to do any cutting. I went through alot of end mills before I learned my lessons.

Regarding the "Power-Curve" of the 770 mill; it's true what has been stated but there is a point where you can get the same amount of torque from the bottom belt position as you can from the top belt position. According to the "Power-Curve" feature on the HSMA software, it's around the 4000 rpm that I don't have to worry about changing my drive belts from one pulley to the other. When I adjust my DOC's and WOC's using this general RPM I don't have to change my belt from top to bottom or vice versa.

The shallower cuts I'm having to make at a slightly faster pace in my 1018 stock means I'm still not completing my parts as fast as I'd like but the trade off for me is that I'm now using more of cutting edges of my end mills and I'm not having to buy new ones nearly as often.

MetalShavings

[ccski]

Thanks all for the comments. I believe that I probably made several mistakes.

Belt was on high RPM could have gained some torque using lower pulley, maybe when machining steel just always use the lower pulley to save me future aggravation.
DOC at 0.080 20% of diameter, maybe limit to 10% of OD in future with full slotting.

Have a much bigger project coming with major pocketing in 1018, 1"x3"x 0.75" deep. Plan was to helical in with 3/8 roughing bit but worried now, maybe pre drill and plunge.

[pickled]

Go to low RPM range and you will be able to make that cut at a slightly reduced IPM. I have run 0.25" slots in 1018 and normalized alloy steels via taking 0.10" DOC passes at 12 IPM with the 770 and a 3/8" 4fl carbide EM. I was using a TIALN coated variable helix EM coupled with fog coolant, but it got these done without complaint. Now did you ramp into the material or just use the center cutting EM to plunge to depth at reduced IPM before you went forward with the X and Y at the IPM you stated? If I have to drill holes in the part anyhow I typically pre-drill a small entry hole to help things out before I slot the material. If you aren't already be sure to get the air pressure up high and pointed optimally to clear chips from the slot or else the re-cutting will sap you pretty fast. Good luck!

[Bryan Turner]

I have a 770 also, for hard materials I would suggest 1/4" 4fl carbide endmill.

I've not tested these, but they look about right. Reduce DOC if you bog down.

1/4" 4fl Carbide, 3970 RPM, 13 IPM, 0.1" DOC, 0.25" WOC; MRR = 0.27

3/8" 4fl Carbide, 2650 RPM, 15 IPM, 0.1" DOC, 0.375" WOC; MRR = 0.51

I would also suggest drilling a larger entry hole and using HSM instead, I find it more forgiving in hard materials.

(also untested)
1/4" 4fl Carbide, 5300 RPM, 73 IPM, 0.46" DOC, 0.021" WOC; MRR = 0.75

--Bryan

[ccski]

Travelling all week so just catching up on the posts.
Next week I will put to use some of the suggestions. Thanks to all who commented, hope to have some good reports next week on the attached!!

[joeyjrc]

I cut 4140 alloy steel with my 770 a lot and I've found its worth starting out with a carbide roughing endmill to get material out quickly. You still have to take it easy but they cut way faster than a normal endmill on heavy cuts(DOC and WOC). Its worth the tool change, try one. FYI they are not cheap but if you get a good coated carbide roughing endmill it will last, as long as you don't crash it.
Good luck.

[ccski]

Interesting day making my compound slide. First used 3/8 Lakeshore carbide 4Fl rougher, 2000 RPM 10 IPM, 0.1 DOC, 0.25 WOC to cut a pocket 2x8X0.375, tool ran well no chatter, finish was adequate.

Left 0.020 radial and axial, switched to new Lakeshore 4 Fl variable flute cutter using same settings as a finish cut, chatter was unreal, tried upping feed to 15 IPM no difference. Finally put the rougher back in and ran at original settings with no chatter or squeal.?????

Used same rougher bit and plunged into a predrilled hole to pocket 1X3X0.75 no issues. So whats the deal with the chatter? Any idea why the rougher would run but a std EM wouldn't? Struggling with the lack of tactile feel a manual machine gives in dialing in the right feeds.

Dont get me wrong, still stoked I took a slab of steel 1.5X3X8 and made it this far in my first real project


Cheers

[Bryan Turner]

Is the rougher a variable flute?
Is the rougher a corncob or rough/finish geometry?
What's the stickout on both tools?

I find most of my chatter issues are related to workholding or stickout problems. Your workholding setup looks good, so maybe shorten up the stickout on your finish mill?

Also, finish only the side or the bottom, not both at the same time. I run a full-depth profile around the part, but pick the end mill up 0.005-0.01 off the floor so it isn't cutting the floor. Then finish the floor without touching the wall. I typically leave only 0.005" for a finish pass, 0.02" seems heavy to me?

--Bryan

[ccski]

Thanks Bryan, rougher was corncob type 30 degree helix. Finish EM variable flute. Today doing dovetails found the tool pulling out tightened drawbar quite a bit so maybe that was part of the problem.

[ccski]

All done, dovetails cut here,later the lead screw and QCTP hole done. Works great.
Learned a ton thanks to all for their comments. Cutting rates and times were way slower than I am sure some could use (few hours of small cuts) but got it done. Not sure if any prettying up will be done eventually but lathe is functional now and I can make round parts too!!

[pickled]

That looks clean and true....good job! Now I bet that you will tackle all sorts of new designs based on this success. That's way cool! I tell you what- of all the jobs and parts that stick in my brain the "FORCED" stretch learning curve ones always come to mind first! You will hear folks reflexively state that they have X years of experience in some field. I definitely value experience and seat time in any "trade" like this. I will say, however, that I have a very high admiration for those that can tell me over X years of experience how many dragons that they have had to successfully slay due to an external (or burning intrinsic) factor forcing them out of their own comfort zones to succeed. Don't get me wrong I love and practice process optimization, but process adaptation/re-invention is TOUGH!

Knowledge acquisition and transfer is such a broad topic, but I can say that I am sad that the notion of apprenticeship has went to the wayside versus becoming ingrained with our newfound borderless communication systems :-(. Maybe we are doing the new knowledge transfer norm here and building for the future? Sorry to derail or detract from your own success/growth, but the iterative nature of this post has fostered this dialog. Wow us with the next level because you definitely have the skills to do it!

[ccski]

Pickled:
I like the "dragons slayed", how true that the stretch provides the growth.
Yes the current state of hands on isn't like it used to be. I did everything myself when young because I had more energy than money, but it's not dead. My oldest never showed a lick of interest in the shop, auto, home repair etc.. Then he got married, bought a house, had a baby and voila... Mr fixit, even makes furniture now for pete sake, never saw that coming.

Guess the thing is, even when you dont think they are learning you are still teaching.
Cheers

[pickled]

That's awesome! I hope that my own son's curious nature draws him into this world so he "gets it". If not maybe he can pick up some of it by Osmosis :-)...hopefully not my frustrated language, but some actual techniques.