[pertierr]

Hello,

I apologize for the length of the post and what I'm sure are dumb questions!

I am relatively new to machining and use a PCNC 770 with the ATC, enclosure and flood coolant. We machine 6061 Al parts < 4"x4"x2". I have been getting back up to speed after a hiatus and realized that I still have these lingering questions. I was hoping to get input from more experienced folks:

1.Breaking bits
We use Solidworks CAM and have been letting it pick the F&S. I find making deep pockets with anything but big mills problematic, and I just broke another bit recently. I was trying to make a 20mmx20mmx15mm pocket with a 3/16 4FL flat end mill, it was one of the HSS China millsets. The flood coolant was active all times aimed at the tool tip. The center pocket was about 15mm deep, and due to previous issues I made the entry a spiral and limited the cut to only 1mm, which seems like it should be safe. The machine got pretty far in(~10mm) and then the bit broke. Here are my thoughts so far, I would love to hear what others suggest:

The first thing I remembered while researching is that I should be using a 2FL bit for aluminum, so I am planning to try a similar feature with a 2FL 3/16 cutter.

When I look at the very tip of the broken bit, it looks like there is a small amount of melted aluminum stuck to the end. I thought maybe the chips did not get cleared despite the flood coolant, so on the next test I will try compressed air as well.

2.PCNC 770 Spindle speed/power
We have our belt in the 'low' setting. I find I have to dramatically slow down the feed on any plunge/spiral because the spindle easily gets bogged down. This has been hard to predict and I've been mostly experimenting with what works without breaking a tool or making the work incredibly slow. I was wondering if others have the same issue. I've been wondering if we should move our belt to the 'hi' position and maybe higher RPM will solve this issue.

3.Coolant system
I find that during every part, the coolant flow starts getting weak and I have to pour more coolant in to restore the flow. We did have leakage issues with the enclosure but we have fixed those, so I can only imagine the coolant is evaporating or sitting in the chips. We have a bunch of containers with mixed coolant and every part it feels like we are just sitting there pouring coolant into the thing. Is this normal?

4.Tool length error
We use the Tormach ETS, and usually set it on the mill table and touch-off the entire tray before starting. Despite this, I find that I cannot use 2 tools on one face. For example, often we will want to rough with a big mill and then switch to a small mill to contour out boss details. If we do that, we can see a significant 'step' between the features. The step is large enough that it cannot be removed with the typical vibratory tumbler processing we do(we use the green pyramid media). We have several theories.

One thought is that our ETS is just sitting on the table or work blank, and the Tormach ATC somewhat 'slams' back and forth, possibly slightly moving/bouncing the ETS. We are wondering if a bolted down ETS is a necessity, it is on our list to try.

Another possibility is that this is just inherent to the accuracy of the ATC system and if we want a fine face finish, then it must be finished with 1 tool.

We also thought the tools might be sliding in the collet, but we have tightened them on a vise and anything further seems excessive.

5.Tool comp question
I spent a lot of wasted time getting up to speed because when I exported g-code from Solidworks CAM, the paths were incorrect in PathPilot. After a lot of diagnosing, it seems the default state of Solidworks CAM has the CAM computing the actual tool path(with the tool size taken into account), but it also defaults to having 'cnc compensation' (G41/G42) enabled. This was resulting in gcode that is compensated twice for the size of the cutter. I still don't understand how can this be the default state and keep thinking it must be some sort of user error, any thoughts on this?

6.Mill setups in g-code/pathpilot
We have multiple mill setups for each face of the part. If we just post the code in one file, PathPilot errors saying that the coordinates are outside the maximum range, because it doesn't seem to know that the different mill setups involve part flips. We have been working around this by posting 4-6 separate files, one for each face. Is this what everyone else does?

7.Carbide mill bits
We are considering getting carbide mill tools if we move the belt up to the 'high' position. Can someone recommend quality sources/tools for making 6061 mostly prismatic parts on this 1hp machine? We find a lot when searching but we don't know what the best tool would be. Our goal is to make the parts faster and also break fewer tools although I'm not sure carbide is going to help with that.

Thanks in advance, and thanks for taking the time to read!

[Algirdas]

1. Check the cutting speed with tool tip data for this material. For soft materials as aluminum is you need very sharp tooltip. Ask your tools supplier for recommendations. With some aluminum alloys the diamond tip is the best. Use your load monitor to get warning before tip and part damage.
2. Again: check the cutting speed of the tip for that material.
3. Yes, it's normal. Look to the chip conveyor catalogs and you will find out how many solutions are there to save colant.
4.
5. Congratulations. You did great research. My advice use the only single compensation at the machine ( G41 / G42 ) whenever possible ( simple 2D shapes ). This enables to change cutter radius compenssation easy without recalculating all the part program.
6. No. Some controls have better solutions.
7. Sandvik, Iscar, Mitsubishi. Ask your dealer for recommendations. Read on-line catalogues - a lot of usefull information there.

[shred]

If you are breaking HSS bits, you'll break carbide as well. Figure out what's going wrong (and it's not just 4fl vs 2fl) and fix that. Chips welding to the cutter mean wrong F&S. Bogging down the spindle means wrong F&S. A lot of your issues sound related to wrong F&S.
.
I downrate standard calculated F&S quite a bit for a non-rigid machine like the 770 because a lot of calculators assume you have a multi-ton metal muncher and want to optimize how much metal you remove in the lifetime of the cutter (which can be as short as 30 minutes in industry). Unless you make lots of low margin parts for a living, your priorities are probably different.

If you have an ATC, run finishing passes with your small endmills and use bigger ones to clear material. Do an axial finish pass and you'll hide the length-variation issues as well.

I make separate files for separate mill setups. I don't like the machine running any code (if only spindle stop, feed hold) while I'm sticking my hands in there. If you run more than one part at a time, run all of one side, then switch the code, change the setup, run the next op, and so on.

High quality carbide can be pushed harder and makes nicer cuts, but even the cheap (not rock-bottom priced) stuff works much better than HSS in these mills. Carbide is less tolerant to abuse, so learn to set F&S before jumping to carbide or be prepared to break a lot of small tools.

[pertierr]

Thank you both for the replies, this has been very useful already. I did not realize that the rigidity of the machine had such an impact, but it makes a lot of sense now that I think about it.

I did some more digging into the solution that Solidworks CAM(CAMWorks) came up with. The cut operation was effectively a slot with a 1mm cut depth on each pass and 3/16 flat 4FL HSS mill on 6061 (T651). The Solidworks CAM F&S library maxed out the spindle at 3250rpm and set the feed rate to 647mm/min (25.5 ipm). Does this seem too fast on the 770? I played around with the settings and one unexpected(to me) thing I noticed is that if I increase the cut depth arbitrarily, camworks doesn't change the feed rate.

I tried online calculators and I downloaded G-Wizard. Some online calculators give a similar estimate to camworks, others give a more conservative rate that is about half(!). For example, the FSWizard iphone app tells me 330mm/min.

G-Wizard gives 523mm/min at 'full aggressive' and 130mm/min at 'full conservative'. G-Wizard seems like a very thorough tool and I think I will keep on using it, but still that seems like such a huge range.

I guess there is no getting around just experimenting within these ranges. Does anyone use any tool in particular for the 770, for example G-Wizard and one particular aggressiveness setting? Or did you pretty much build your own spreadsheet through experimentation?

[shred]

Thank you both for the replies, this has been very useful already. I did not realize that the rigidity of the machine had such an impact, but it makes a lot of sense now that I think about it.

I did some more digging into the solution that Solidworks CAM(CAMWorks) came up with. The cut operation was effectively a slot with a 1mm cut depth on each pass and 3/16 flat 4FL HSS mill on 6061 (T651). The Solidworks CAM F&S library maxed out the spindle at 3250rpm and set the feed rate to 647mm/min (25.5 ipm). Does this seem too fast on the 770? I played around with the settings and one unexpected(to me) thing I noticed is that if I increase the cut depth arbitrarily, camworks doesn't change the feed rate.

I tried online calculators and I downloaded G-Wizard. Some online calculators give a similar estimate to camworks, others give a more conservative rate that is about half(!). For example, the FSWizard iphone app tells me 330mm/min.

G-Wizard gives 523mm/min at 'full aggressive' and 130mm/min at 'full conservative'. G-Wizard seems like a very thorough tool and I think I will keep on using it, but still that seems like such a huge range.

I guess there is no getting around just experimenting within these ranges. Does anyone use any tool in particular for the 770, for example G-Wizard and one particular aggressiveness setting? Or did you pretty much build your own spreadsheet through experimentation?

I use FS Wizard for starting points on unfamiliar material, then dial it way down at the machine with the feed rate override to start with and gradually speed it up to where its happy. Then I save that in my CAM as the next starting point. No particular reason to chose FS Wizard except I'm used to it.

The root problem is unless you use the same setup and same tool length and depth of cut and everything for the next part, you will probably need to tweak it again. Some materials have a very narrow range of speeds they like to cut at, some like aluminum don't care as much. Once you're in the ballpark for speed, adjust feed to match what your machine likes to do.

FS Wizard and G-Wizard try to take into account spindle HP and tool flexing, but don't do as much for machine flexing, so run conservative on their numbers. Until you get to chatter or process cycle time becomes important, a little conservative isn't going to hurt anything.

FWIW, 25ipm with a 3/16" HSS cutter at 3200 RPM seems aggressive to me, although I don't do much with HSS so don't have a good feel for it off the top of my head. Maybe someone else can help with that.

[dazp1976]

I did some more digging into the solution that Solidworks CAM(CAMWorks) came up with. The cut operation was effectively a slot with a 1mm cut depth on each pass and 3/16 flat 4FL HSS mill on 6061 (T651). The Solidworks CAM F&S library maxed out the spindle at 3250rpm and set the feed rate to 647mm/min (25.5 ipm). Does this seem too fast on the 770? I played around with the settings and one unexpected(to me) thing I noticed is that if I increase the cut depth arbitrarily, camworks doesn't change the feed rate.

I find slots are a different animal altogether. Generally I have to half everything.
I have best luck with 3fl cutters. They give the best of both worlds, the evacuation of a 2fl & the rigidiity of a 4fl.

[kstrauss]

If you are having problems with chip welding using tooling with the appropriate coating will help. I've had good luck using carbide with ZrN coatings.

[Algirdas]

Try to increase the chip thickness. This will increase heat removal rate.
You need to take into account the cutting speed fot that aluminum with that tool tip. The selection of software to calculate rpm and feedrate is far away from priorities.

[AUSTINMACHINING]

Don't use a slotting tool path unless you are making a slot. If you have to slot, shallower faster cuts unless you have fire hose flood cooling. No such thing as too much coolant in aluminum. Chip evacuation is a lot harder in slotting operations. Use adaptive clearing whenever possible. If your profiling 2d parts(slotting), use tabs so when you break through, the part and the stock are connected. A floating piece of stock is a 90% chance of broken end mill.

Carbide or HSS. Sharp is the key and the cheap chinese stuff is typically horrible.
Suncoast tool sells YG1 alupower 3 flute end mills. Reasonable, carbide, and crazy sharp.

HSM advisor is great for F&S.

[pertierr]

I just wanted to say thank you for all the suggestions. I changed to carbide mills, changed the belt to hi and started using HSMAdvisor instead of the camworks F&S library. I have made several parts with deep pockets with no issues and the finish is so much better than before. I have been running HSMAdvisor on the '0.5x performance' to get conservative values and that seems to work great on the Tormach.

There is one remaining nagging question/observation. As I mentioned above, I have HSM Advisor set to the most conservative setting. Even then, I have reduced the plunge speed from what it says because traditionally that has been challenging on the 770. However, it still seems to slightly slow down when plunging. Let me give an example, on 6061 with a 1/2" 3FL carbide CrN coated for a 1mm plunge and slot HSMAdvisor says 8309 RPM and 407 mm/min plunge feed(I have the plunge RPM locked to the normal RPM). I set a much lower 150mm/min Z rate and still there is a slight slow down and chirp when it is plunging. It almost seems as if the motor is not providing 1HP but something less than that.

[dazp1976]

However, it still seems to slightly slow down when plunging. Let me give an example, on 6061 with a 1/2" 3FL carbide CrN coated for a 1mm plunge and slot HSMAdvisor says 8309 RPM and 407 mm/min plunge feed(I have the plunge RPM locked to the normal RPM). I set a much lower 150mm/min Z rate and still there is a slight slow down and chirp when it is plunging. It almost seems as if the motor is not providing 1HP but something less than that.

That's about how fast I plunge on my PM25.
Tbf. If I am slotting at 1mm deep I ramp in both ways at 0.5mm, normally it's with a 1/4" bit though.
I actually only have 2500rpm on mine and I feed at 400. Ramps 0.5mm one way, 0.5mm the other, then a level pass.
At 8000rpm, one would technically expect to get at least 800mm/min with this method. Maybe more using a more rigid 1/2"

I run a 1/8" using the same method but only get a perfect slot at 315mm/min with 2500rpm.

It's all about finding workarounds to machine limitations that may seem daft on paper but are less agressive and turn out to be quicker.

[snovma]

For smoothest way of handling and sorting products for further processing and packaging I would highly recommend you vibratory bowl feeder. For example, for my sweets products I ordered it from here https://www.sandfieldengineering.com.../bowl-feeders/. They have a large variety of bowl feeders (types, sizes, etc.) Also they provide a complete range of services and equipment associated with bowl feeding components like hoppers, belt conveyors, loaders, and controllers.