Home shop guy tries again with G-Wizard

Having licensed the most recent version of GW and watched the two videos, I felt "enabled" to try again. Now I wanted to do a facing cut in CRS to a depth of .300".

GW suggested a 48% radial engagement, 2600 RPM, and 23 IPM at full DOC with a 7/16 carbide endmill and 1/38 "stickout". So with trepidation I plugged those numbers into CAM and single stepped through the first two cuts. I found that the noise (squeal) was really loud although the finish (not a critical factor) was fair. The bad part was that the end mill pulled out of the collet slightly on the second pass, which was conventional milling (I was using a back and forth cut pattern). So now I have a ramped cut and a too deep DOC on one side.

So the first question for the forum is why the collet pulls out on the pass using conventional milling, while the first pass using climb did not.

Although the part is now unuseable, I decide to continue to try different options. This time I really cranked down on the drawbar. I reduce the DOC to .100 in GW with the same radial engagement and get 3056 RPM at 23 IPM. I plug this into CAM and run it single step for a couple of passes. Chatter is now gone or pretty minimal in climb milling, but is perceptible in conventional. So I modify the CAM settings to do each pass in climb and run the program to completion. The results are very satisfactory as to finish.

The remaining question re this part has to do with the lead in move. I had specified a tangential move on each pass, meaning a G3 from outside the part to the start of the next cut. This move had the same feed rate as the rest of the cut. So I am now wondering if the move that enters the side of the material needs to be (significantly?) slower in order to not shock the endmill. It did seem to have a somewhat louder sound on entry vs. the longer G1 that follows.

Thoughts?

I think you may be pushing way to hard.
I would look at about 500 sfm (4300rpm.) & about a .003" CPT. Assuming a 4 flute, that would be about 50" a min. However, your "ae" should be 1 x dia. with a 5-8% stepover, climb cut only.

As far as your endmill pulling out on the convintional pass. It would seem more logical for it to pull out while climb cutting, but your collett may have just come loose on the pass back.

GW computes chip load as .0019 and 350 SFM. My mill has a max spindle speed of 4000 rpm. Endmill has 4 flutes.

I just downloaded a trial of G Wizard and entered your parameters of 7/16" Carbide, 4 flute, 48% engagement, and .3 doc in 1045 steel and it gave me 1881 rpm at 13.04 ipm. Chip load was .0017".

kvom01 said:

Thoughts?

Click to expand...

I think you are seeing the limitations of your machine.
I would try the same cut, but back off on the radial engagement to maybe 25% and make the cut in 2 roughing passes and then a finish pass. See what happens. This is only a 1200# machine.

As for the collet issue, you should not have to "really crank down" on the drawbar. The tool slipping may be just an indication that you can't make a cut like this. Or it might just be a crappy collet...

Glenn Wegman said:

I just downloaded a trial of G Wizard and entered your parameters of 7/16" Carbide, 4 flute, 48% engagement, and .3 doc in 1045 steel and it gave me 1881 rpm at 13.04 ipm. Chip load was .0017".

Click to expand...

I assume he is using a low carbon steel...I don't think he said otherwise.

OK

2 problems as I see it. One is that GWizard has some funny behavior in this scenario. The other is that you need to really do a reality check before you run your parts, but you need more experience to know what will work.

What happened is that you wanted to mill .3 in deep so you loaded the parameters into GWizard at .3 deep and asked it to determine the width for that depth. The problems is that there is NO width that will work for that depth and it gave you a warning, but you didn't see it. Then it still made up a number for width, instead of giving you 0, it gave you .2127. That is a bug in my opinion, but we will have to see what Bob has to say about it.

What you needed to do was back off the depth. I tried .15 in and it gave me a reasonable width of .2782. As you gain experience you will know what combinations will work. Bob has made a pretty nice tool, but experience will really make things work better. Hang in there.

Bob needs to look at this....
With the optimizer open, I changed the tool stick out then hit the optimize button to recalculate. This is with holding the depth at 0.3" and letting the optimizer pick the width.

At 1.5 it succeeded
At 1.38 it failed (The stick out in question)
At 1.28 it failed
At 1.21 it succeeded
At 1.14 it failed

GW changed the width of cut for each tool stick out above. But if it finds a good cut width of cut for a stick out of 1.5" why did it not find a good width of cut for a stick out of 1.38"?

My info so you can replicate this:
Depth 0.3"
Tool dia: 0.4375
Width of cut: given by the optimizer.
Carbide endmill in 1020 steel


To the OP: this is still not your problem. A 7/16" carbide EM can easily cut .3" deep with your small stickout. Strongest bet is that your machine is not rigid enough for the cut you are taking. You gotta learn what your machine can do and what it can't. And always keep the work set up as rigid as possible.

You guys have found a bug, thanks!

There is a slight difference in the rounding between what the optimizer sees and what the code that checks to see if it succeeded sees. So the optimizer finds a "solution" that due to the rounding error the checking codes says is not a "solution". The difference is in tenths, so in fact there really is a solution, but the two should agree or it is confusing. I will do something about it in the next release.

Let me think about whether to have the optimizer get in your face more if it doesn't think it got a solution.

Getting back to the OP's issue, let me offer some thoughts:

First, on the collet pull out, it's an issue some folks have and no fun. I hate running R8 collets and have essentially quit a long time ago. I use only solid holders because they're repeatable w/o something like TTS and they seem more rigid. My use of a powered drawbar also ensures consistent torquing, and it is nice to have as many variables be stable as possible.

I do like to use ER collet chucks unless roughing with an EM 1/2" or bigger where I will use a setscrew holder. People are surprised at how much torque collets need. I think Tormach is publishing or has published an article to call attention to the requirements of it because they've had a lot of calls about collet pull out.

Why would the conventional pass pull it out while the climb didn't? I can only offer the thought that the climb might have pulled it out slightly at which point it gets worse. A little slip makes a deeper cut which increases the forces which makes a deeper cut, yada, yada. Ugly cycle.

Another issue is the difference of force in the two types of cut may have contributed. In climb milling, most of the vectors will force the cutter closer or further from the cut wall. In conventional, they force the cutter along the direction of travel. There is a picture on my page here:

Machine Tools: Feeds and Speeds, Mill Cutters & Surface Finish

Looking at the picture, and only considering those vectors, I'd conclude to keep the deflection as light as possible when climb milling as the direction of deflection will impact your accuracy. But, when you were conventional milling, the tool likely deflected back along direction of travel. This may have allowed it to "fall behind" the feed a touch which wouldn't make it happy and might have helped drag on the collet's grip.

The chatter also bothers me as depending on how much vibration there was, that may have loosened the drawbar if it wasn't real tight. I try not to run cuts that chatter continuously, a little bit in the corner maybe, but not the whole pass.

My bet is on it having started to slip a bit even on the climb pass.

Okay, what can we do differently?

First, save that cut in your Cut KB so it is there to refer to as one that didn't work.

Next, consider some experiments to see what will work. You have to get it to quit pulling the tools out of the collet before anything else, then you need to eliminate the chatter. Certainly try torquing down the drawbar tighter. If you have any solid holders, try one of those. Be sure collet and tooling is clean. Oil and chips will degrade the collet's holding in a hurry.

For the chatter consider both reducing and increasing the cut parameters.

Chatter is a resonant phenomenon. People's instinct is to slow down, but it's just as susceptible to speeding up. The reason is that you're trying to move out of the resonant frequency where its occuring and you can move either way to get off that frequency.

If you have feedrate and spindle override, it's pretty easy to play with it. I always try increasing first. Try feedrate first and then spindle, because you don't have a very wide range of spindle rpm. On a VMC with a 10K spindle, you can try spindle first if there is room.

You can also try to tune away chatter by changing the tool stickout. 0.200" of stickout change is enough to start to affect it, but is usually little enough not to radically change rigidity except for small tools. This practice of adjusting stickout to get to a more desirable rpm range is called tool tuning.

You record all these experiments in the Cut KB and they'll be there to help you next time you want to do a similar cut. In the longer run, G-Wizard will start to get smarter by watching what goes into the Cut KB, but we're some months away from that. We'll also be adding some tools specifically to work with chatter so your Cut KB can use the data to produce a stability lobe diagram, for example.

Last point. That cut was a 1HP cut (I think?). That shouldn't be too much for a 1200lb mill, but there will be some limit. If your mill is lighter, it may be less. If heavier, may be more. There will be some number where things are almost always comfortable. That's not the point of max production efficiency, but for a home shop guy, that doesn't matter. For those users, you can dial back your mill's HP in GW. If 1 HP is fussy, try 0.9 HP.

GW automatically scales back the cut to your HP limit, so setting one will help keep it from getting too aggressive. This is a better way than using the adjustment factors on SFM or chipload.

Best,

BW

I think I'm getting a handle on it now. With 1-off parts speed isn't that critical, so I think backing off on DOC and using GW for S&F will likely keep the tools from breaking.

I would still like opinions on whether lead-in feed rates should be slower than full cuts.

i would be careful as to what gwizard has to offer on the cuts. i would first look at what niagara has online. if you got to Niagara Cutter - World Leader in Thin Film Coated End Mills, Milling Cutters, and Carbide Tools. under their tech section they have recommended speeds and feeds and doc. now ultimately each end mill is different, but at least you can get some general parameters to start with.

SD, I a going to assume you have never used GW before as you don't seem to understand how it works.

If you use Niagara EM's, you *SHOULD* plug Niagara's data into GW. It's not hard to do. Put it in a spreadsheet and import it. Send me the spreadsheet and soon others will be able to import it too. You can see how it works and what's available here:

CNCCookbook G-Wizard Custom Tooling Data

Think of G-Wizard as being a way to add value to whatever tool data you have from your manufacturer, and as a source of data if you don't have any. The data it uses by default is relatively conservative. It's derived from an analysis of a large number of manufacturer's data.

How would it add value if you have your manufacturer's data?

There's just a heck of a lot more that can be done with feeds and speeds than the simple formulas we learned will do. In fact, many times those formulas can be downright misleading, for example if you're cutting less than half the diameter radially you need to compensate for chip thinning. GW does a whole ton of those types of compensations automatically: chip thinning, ballnose, hole depth for bits (e.g. it'll tell you when it's time to peck, when a parabolic is preferred, and so on), adjustment when slotting with tailoff for increasing axial or radial engagement, interpolation between table data values, adjustments for material hardness based on condition, and on and on.

In the end, it's all about how many variables you can master. Data tables only manage a few. You just can't lay out 10 dimensions worth of tables on a page! Niagara actually lays out more than a lot of manufacturers and their data is part of the master collection that determine's GW's defaults, BTW.

Aside from mastering the variables, its also all about getting past even the manufacturer's data. The manufacturer has to give you conservative feeds and speeds because it doesn't know your shop, your best practices, or your job. This is one reason HSM toolpaths can go so fast--one more variable got controlled and known--the tool engagement angle.

In the end of the day, best feeds and speeds turns into an empirical game. You have to find the edge of the envelope for your machines, holders, particular brand of coolant, and other best practices. That's Knowledge Based Machining, which is something added fairly recently to GW.

Cheers,

BW