If you’re cutting deeper than your LOC then you will certainly run into issues unless you have a reduced-shank endmill, which the spec sheet says is not.
The shank part rubs on the material like piloted router bit, keeping the cutting edges away from the cut and bending the tool.
That is what I thought. If I want to reduce the thickness of the gear to be better suited for the end mill with an LOC of .375 inches, would you make the gear like .342 inches thick so the end mill can overlap the top and bottom by .004”? Does that make sense?
Richard
PS: I think the reason the longer end mill is not working is probably because when I first started the project, I did not have it choked up enough in the collet. I machined a gear and had lots of chatter. I ended up chocking it up about .100” inches into the collet, but I am guessing that I may have damaged the end mill when I machined the first gear.
You’ll need to play with max-LOC per endmill to see what will work and have good chip evacuation.
Get a good strong magnifier and have a close look at the cutting edges of your endmill to see if it’s chipped or worn. I mostly use a 10x eye loupe but occasionally get out the inspection microscope for tiny ones.
Thanks Roy. The best I have is an 8x loop and it looks fine. I am going to do some tests on a straight-line cut and see what happens.
I just realized that I am chamfering the top and bottom leading edge, so I can get away machining close to the full LOC of .375”.
Best… Richard
Do you cut the inner spokes first?
If so, try them last. Extra material in the disk will dampen vibs a bit and provide more rigidity. Even with the material left on the bottom, its a bell looking to get rung. Is the workpiece clamped down somehow or is it a vacuum table?
As to why the longer 1/8” EM didn’t perform, I think all would agree on not choking it up in the toolholder → chatter
You had a thread a while back asking about feeds and speeds. What software are you using to calculate feeds and speeds?
Of the options discussed on here in various threads, IMHO, after purchasing Millalzyer, the author can import the 1500MX CAD model and that would give you the best chance at modeling optimum parameters compared to FSWizard or GWizard once you get past the learning curve. Probably as close to getting “tap test” as you can get without buying the hardware if the actual machine geometry is being used in F&S simulation/calculations.
I have to wonder if that EM is also not too happy as it could be in a 10k RPM spindle given it is designed for a 2-3x speed spindle and it ends up outside of the performance envelope where you have to slow it down even further than calculated. Just a shot from the hip there. I haven’t run the math myself to confirm.
In terms of process analysis, my optimal process for my anemic 440 is to put the full specs of each EM into a calculator and use the software tool to evaluate cutting parameters that will be fed into Fusion CAM. Ideally, I end up putting together a couple of F&S presets that depend upon the DOC to pick from for the operation being performed and the max DOC required (I guess the two cases I work from are adaptive higher MRR vs. contour/finishing). It’s not optimal compared to a “professional” approach to CAM.
I have access to CloudNC but apparently their installer has gone bad and doesn’t cooperate with MacOS. I submitted a bug report and they are aware of it but have yet to solve the issue two-three weeks later. So much for AI assisting software engineers to help them squash bugs quicker…
I’m looking at going away from all the more one-off programming to spending a little more time on my next couple of CAM layouts to build out a more programmatic approach which was outlined in an Autodesk webinar some time ago where in theory, I can drop a part into an overall assembly with existing CAM that will pick up on part features and reduce having to build out CAM manually.
I have to think about marching the gears first as the bottom stock is still supporting them. Still worth a try… Thank you!
For what it is worth, I have never had issues with speed and feed before. I have probably machined a 100+ parts at this point. I usually start with 70% of the MFG spec sheet and use GWizard with no issues at all. My humble opinion is that there is something strange with this end mill, especially when any combo of F&S I threw at the YG1 worked great. Unfortunately, they don’t make one with a .5” DOC.
I tested this weird end mill today on a 4” straight run of aluminum, iterating from the 5000 rpm F&S that worked and crept my way up increasing rpm, then feed rate and landed on the following:
Roughing: 7000 rpm, .2 DOC, .04 WOC and 15.4 imp.
Finishing: 8000 rpm, .2 DOC, .004 WOC and 24.5 imp.
Both of these left a chatter free surface but neither compete with the surface finish from the YG1. Most likely due to the fact that it is coated. Increasing the rpm further for either of these recipes resulted in the start of diminishing surface finish. Who knows, maybe I am making something from nothing, and I am just used to the surface I get with YG1 end mills.
I am still deciding between modifying these gears to accommodate the YG1 end mill or trying again with this end mill.
One question: In fusion, feed optimization shows up on the tool paths as the part of the path that is slowed down turns yellow. I did not see yellow in the tight radius of the gears. Can anyone let me know how to modify the settings so it works correctly.
Thanks for all your thoughts… Richard
One more fun game I play when trying to perfect surface finish is cranking the feed knob while cutting. It helps if you make marks on the part before or have a photographic memory. What I do is on the finish pass, just pick a point and slowly turn down the feed maybe 20%. Then once you get the feed down 20, then at the same rate turn the rpm down 20%. This should give you 2 segments to compare and you can figure out the rest from there. This can allow you to isolate a lot of harmonics. Sometimes it leads to really beautiful patterns as well. I have been trying to get perfectly smoother finishes and discovered beautiful fractal surfaces instead. The thing about harmonics in these machines is that they propagate and reflect differently depending on how the work is held, the shape of the remaining material and the shape of the cut as well as the frequencies generated by rpm and end mill shape. So if you get something you like it has to be exactly the same to repeat. It sounds like a lot but it’s all logical in a scientific way.
The FSWizard web app is free for anyone to run calculations (I don’t think it lets you store a tool library in the free version, I have HSMAdvisor, so that function is included for me on FSWizard, which is my go-to for a quick F&S calculation).
Anyhow, it spits out different feed numbers for that GWS EM if I use the RPMS/DOC/WOC that worked for you without chatter (unless I’m out of practice and am not remembering how to use it): 87 in/min finishing and like 10in/min roughing. I have enabled the HSM and Chip Thinning adjustments for those calculations.
If I don’t specify RPMS, it wants to run it at 10k if I specify that as the max. If I tell it the spindle can spin to 35k, it will try and spin it as fast as it can and at a high feed rate, as per the manufacturer’s chart.
FWIW, I paid for a GWizard license and I stopped using it not long after I started playing with it and HSMAdvisor/FSWizard at the same time where I found HSMAdvisor/FSWizard to be more intuitive for me.
GWizard is quite buggy, and there was essentially no technical support even before the developer passed away.
Guys, thanks for all the tips. Here is the bottom line.
I spoke with the folks from GWS Tool Group/Monster and they said that Suncoast Tools sold me the wrong end mill. This end mill is specifically designed for very high rpm. It is really happy at 20,000+ rpm. Running it at lower speeds which results in higher torque is not advised and will most likely break the end mill.
I reduced the thickness of the gear so I could run it with myYG1 end mill. I ran it with the originally suggested feeds and speeds, and it ran flawlessly. Not a squeak or chirp to be heard, and I got the usual mirror finish I am used to from the YG1 end mills.
I really appreciate all your thoughts. Bruce, thanks for the tip on cutting the inner spokes last, while it was not necessary on this one, I will certainly keep that idea in mind.
With respect to the feeds and speeds, GWizard is certainly a bit clunky. To be honest, I used it more with my previous benchtop mill, but I am finding that the Tormach 1500 dampens vibrations so well that I have more latitude nailing the F&S. It is way more forgiving. For the most part, I have been using the YG1 suggested F&S, starting at 75% of their values and adjusting based upon work holding etc. Since I am a hobbyist, I’m more concerned with getting the best surface finish and keeping an eye on chip thinning. If the part takes 2-3 minutes longer to run… not really a big deal.
Thanks again… Richard
YG for the win 
After using one alumax years ago I changed all my tools for aluminum over to them.
Whisper quiet and decent finish.
I use hsm advisor for feeds and speeds and also to provide good numbers for threading using lathe or single point threading on mill.
Glad to hear you got this sorted out. That’s sort of what I was thinking with the recommended speed range being 20-30k.
I had a similar issue happen to me with an indexed roughing EM (that is probably a little too aggressive be using on a 440). I was puzzled at the issues and then I did the same as you by running a controlled pass and found it was cutting wider than expected. The EM manufacturer quickly responded to my call and requested I ship it back for inspection. They promptly sent me a replacement as the confirmed it has slipped out with the wrong inserts.
Yah… I didn’t think running an end mill slowly could cause issues.
Funny, I called the YG1 representative Bill Pulvermacher who always gives me great insights. He has over 40 years of experience and told me that a good rule of thumb is that small chatter is usually related to the tool, and large chatter is usually the setup. Good to keep in mind.
BTW, the YG1 spec sheets don’t provide info related what ramping angle is appropriate for their AluPower end mills. Bill said they can all handle a ramp angle of 5 to 8 degrees.
Best… Richard
I’m changing all my angles tomorrow! That’s 150% faster than the fusion default of 2degrees.
I’ve always defaulted to 2 degrees as well. I ran 5 degrees on a 3/16 and 1/4 inch end mills today and what a difference. If anyone wants I can pull up Bills contact details.
Machining is a lot like gardening, the answer to every problem is always more, unless it’s less.
The YG/Pulvermacher recommendation is great stuff.
For another take on ramp angle, there is this HSMAdvisor KB which also provided some basic machining knowhow (like, to drill a pilot hole, since a drill is a tool that is meant to do that, where an endmill may not be designed for plunge/center cut). Mostly putting this here for those of us who didn’t go to school for machining and have been picking this up in pieces through the school of broken carbide and eStop emergencies…
Ramp chipload adjustment for 4 flute Center cutting end mills:
0-2.5deg=100% of normal feedrate
2.5-5deg=75% of normal feedrate
5-15deg=50% of normal feedrate
15-30deg=25% of normal feedrate
30-45deg=5% of normal feedrate”