[xanth]

Can anyone help me figure out why I am breaking so many endmills? I've probably spent $100 this weekend just destroying 1/8" endmills. I'm at my wits end.

The attached job in the zip file is for SprutCam 9. I am using a Tormach 1100 (max spindle speed of 5100 rpm). My material is 6061 aluminum. I am trying to take a 1/8", 3 flute, ball nose carbide endmill and cut a 3D profile. The tool has a 1" stickout. Although the shape is double sided, I am only doing one half of the shape and leaving the rest as stock. (This was a "test" shape from another CAD program, and I was able to successfully mill it on my Taig using that program...)

Using GWizard, and taking a cut width of 0.015" and a depth of 0.050", I get a max feedrate of 70 IPM (before deflection becomes an issue). I dialed it back to 68 IPM, just to give a margin of safety. This gives a chipload of 0.001 IPT, which seems very light to me. I realize that in the CAM file, calling this a "roughing plane" is more than a bit of a joke, but I wanted to try this using just one tool, rather than worry about tool offsets and all that jazz, since this is my first time using the Tormach.

Although both GWizard and SprutCam seem to suggest this toolpath is great, it breaks my endmills. What am I doing wrong here?

Thanks in advance for your help!

[tgsell]

When I enter your numbers in Gwizard I get 18.4IPM... Make sure Gwizard is up to date.
What type of cutting fluid are you using?
Have you inspected the broken endmill for clogged chips in the flute? I would tend to use a 2 flute for Aluminum,especially for such a small cutter diameter.


Attachment 289374

[mountaindew]

In my opinion I would start with some simple object models with chamfers, ledges, grooves ,holes and round edges. Import models into sprutcam and practice setting up various mill operations with different tools. Then test above operation sets on some wood or other soft material. Go back to cam and practice changing doc, woc, speeds feeds along with approach other parameters and repeat testing at mill. So much can be learned in just 8 hours of practice doing this. Also it allows the operator to build confidence in the process. Try NOT to focus so much on feeds and speeds and SLOW down and learn the entire process. I started out doing this and avoided broken tools, scrapped material, and tool crashes in general by testing and using slow feeds "under 25 ipm for normal tools and under 10ipm for small tools" with doc , woc always some low percentage of tool size! No need for wizards until you start working with intense or difficult materials. As noted above if you practice and develop a complete process from drawing to part and continue to build your skills in time you will have the confidence to make most anything with no broken tools and scrapped material. Something to consider, its hard to drive a race car at high speed without practice. Most people are going to crash the car many times before they learn the performance envelope. Imho the same applies to using expensive precision tools like these.

note! Starting out with no experience, in 18 months I have broke 2 hamier probes "jogging", couple drill bits "error in tool offset", one 1/8 em "bad tool paths". I also damaged 1 vise jaw and destroyed a 1/2 end mill, not my fault and turned out to be a software bug in path pilot.

[xanth]

tgsell, sorry, yes you are correct! I originally tried with that IPM, but the cutter broke. I had assumed that the low IPT was causing rubbing/chatter and since carbide doesn't do well with either, it was causing the breakage. I took that same screen and dialed up the IPT to 0.003 to get that figure. It was still below 0.001" deflection.

EDIT (forgot to answer two questions): for cutting fluid, I'm using DuraKut 4010. It's what Tormach sells on their website, and it's a water soluble solution. I used a brix meter to check the concentration at around 5 brix. I didn't see any clogged chips in the flutes, but the cutters also tend to bounce all over the closure when they snap off, so that might not mean anything.

I have also tried using 2FL cutters-- one of which was a HSS that had a 3/8" shank. Even after adjusting feeds and speeds, I get the same thing. I'm getting really good at throwing money away.

mountaindew, you have good points. However, I'm a bit leery of using wood in the Tormach. Won't that gum up everything, both the machine and the tools? Also, wouldn't you want to have much higher feeds/speeds for wood? I've used (and made my own) machining wax before, and I found that you can do all sorts of things in material that soft that in no way could you ever do with metals. However, your advice about slowing down is something I'll take to heart... Still, if you can't trust these calculators to not break your tools, what worth are they?

One thing I did notice, it seems that when the endmill comes across the surface of the shape at certain levels, because the material has not been thinned away evenly on both sides (it does part of one side, goes around the shape, and then comes back for the section it didn't do earlier), the tool is actually engaging at 100% cutter radius. That seems to be where it is breaking. However, I can't seem to find any way in the roughing plane operation to prevent this from happening. I know in waterline, we have the options of doing depth first vs level first, and something like that in the roughing plane seems to me like it would solve the issue. Any thoughts? (Also, if that explanation makes no sense, I'll add a picture of what I'm talking about later tonight).

Thanks for taking the time to take a look at my bumbling, guys. It's most definitely appreciated

[mountaindew]

What I was advising will not hurt anything, mill, tools or fixtures. I was suggesting mostly for test profiles and operation refinement until a good process is zeroed in on and your seeing results. Cleaning and adjusting your tormach system is imho another skill that has to be developed for long term use. Dust from everything in shop will be in contact with and foul your mill and fixturing. In short I spend 25% of my time cleaning and organizing all my tools including mill, in the old days we called this roll out and roll up. I must say its easy to get frustrated if you spend a half hour looking for something or hours making something only to find some debris spoiled the setup.

[popspipes]

wood is good in the learning process, I used lots of it.
I also make wood boxes on the machine, the biggest problem is the wood needs to be really dry or it will dull cutters, carbide or hss due to the acids in the wood, otherwise it works fine.

I have a grooving/slotting op in aluminum with a .125 ball mill .125 deep, I run this at 5 ipm and 8 passes, this works and is probably a bit slow but doesnt break cutters unless I dont have the coolant set quite right, once the flutes plug up its all over, 5140 rpm 5 ipm, about .015 doc.

[Strip]

I make a lot of cuts in 6061 with a 1/8 endmill. I almost always cut at 5100 RPM and 10 IPM using 2 flute EM's I have cranked up to 11 IPM and snap. So, I just usually set them all at 10 ipm and .05 to .06 depth and let it run. It takes a while, but way faster than breaking bits. I do suggest you run 2 flute EM's on 6061 and 6063

[awerby]

One thing I did notice, it seems that when the endmill comes across the surface of the shape at certain levels, because the material has not been thinned away evenly on both sides (it does part of one side, goes around the shape, and then comes back for the section it didn't do earlier), the tool is actually engaging at 100% cutter radius. That seems to be where it is breaking. However, I can't seem to find any way in the roughing plane operation to prevent this from happening. I know in waterline, we have the options of doing depth first vs level first, and something like that in the roughing plane seems to me like it would solve the issue. Any thoughts? (Also, if that explanation makes no sense, I'll add a picture of what I'm talking about later tonight).

That would definitely account for the broken tools - you don't want to suddenly engage 100% of your tool radius. It sounds like a problem with Sprutcam; did you figure out how to avoid this yet?

[lincolnrogers]

That would definitely account for the broken tools - you don't want to suddenly engage 100% of your tool radius. It sounds like a problem with Sprutcam; did you figure out how to avoid this yet?

Just thought I would comment that I have also had this problem where machining was all going fine up to a point where Sprutcam would engage a cut with 100% tool radius and break the tool every time. Its made me a little weary and going over the program I could find no way to stop Sprutcam doing it in this particular case.

[popspipes]

What operation are you using in Sprut that is doing this, I didnt see it listed above?
I use sprut 7 but there should be a similar op, just curious as to why its breaking endmills.
I would try cutting the doc to about .020 and 10 ipm, 5140 rpm and see what happens.