Slow motion CNC broken tool

[laurent_parti]

Hi all,

Often we succeed in our project but sometimes not. With this experience I had a leason learned. I prefer to share it with you maybe you can avoid it:

[ame]http://www.youtube.com/watch?v=1moX_dbWxDc[/ame]

Laurent :wall:

 

[kvom]

For me your tool stickout was way too large. Best practice is to keep the stickout as small as possible for a given job, as the tool rigidity is maximized.

 

[jwcnc1911]

Crank the pot man! In my experience that type of surface finish is a result of too much heat. Surface footage is way too high. The aluminum chips are gumming up and sticking to the workpiece. Slow the spindle down or crank the feed way up.

For speed/feed reference this is milling the flywheel for the De Waal rhombic. It's a 0.750in (19.05mm) hss 2fl endmill. 35ipm (889mm/m), 49% stepover, .125in depth of cut, 2800rpm


[ame]http://www.youtube.com/watch?v=nZ5bvLbYbZo[/ame]

Before any one jumps me... I do realize our machines are very different. As I recall we discussed this before. I'm just trying to emphasize the feed/speed relationship. It will cure your surface finish issues and save you money on tools! If you have an Android cell phone download FandS - it's free and has always given me good feeds/speeds.

Hope that helps!

 

[mu38&Bg#]

What were the cutting parameters?

 

[laurent_parti]

Thanks all for your inputs.

Android soft will be a great help.

Parameters are the following:

Tool: 0.12" diameter 2 flutes end mill with center cut
Speed: 7500 rpm
Feed: 31 inch/mn
Deepth: 0.02"
5% stepover :hDe:

And more, after the first layer at -0.02" made in conventionnal travel, the second layer at -0.04 starts with climb travel and 100% of the tool diameter width !

 

[jwcnc1911]

OK... So the slomo video threw me. Your actually going too fast, way too fast. :fan:

Your radial WOC is far too much (on that first step down in the parallel lace operation anyway) I don't know what CAM you use but in a lace operation you should be able to define entry parameters such as helical, 3d path or 2d path options for this purpose. On the pass to go down to the next level you can specify how many steps to take to get to depth.

If you don't have these options you can always machine away material for clearance.

I've really come to dislike parallel operations over the years. Try a spiral path, choose a start point in the middle of the part. You'll never engage more of the tool than you want.

Here's what I get when I put your parameters in:

 

[mu38&Bg#]

I try to run .001-.002" per tooth and I often run ~15,000 RPM. Depth of cut and stepover are somewhat limited by the rigidity of the machine. I usually run 75% stepover, to avoid problems with full width cuts. A very good (expensive commercial grade) CAM would allow me to run the parameters I'd really like, but if I had the money I'd be running a Hass Minimill or similar instead of my frankenmill.

A slotting (full width) pass is always conventional, think about it.

In the video, the aluminum overheated, clogged the flutes, stopped cutting, and broke. With some lubricant it may have made the cut. Depends on the grade and hardness of aluminum and the cutter type.

Have you checked tool runout when installed in the spindle? Too much runout effectively makes your two flute a single flute and the feedrates will be wrong which kills the cutter. 0.5mm DOC at 400mm/min is about all I could do with my old spindle. Another issue is plunge feed rate, this used to kill me a long time ago. If you attempt to plunge at the full feed rate it will instantly clog the cutter in AL.

Did you define your stock properly in your CAM? Maybe it thought your stock was equal to the extents of the part, which means it thought it would be making a small radial cut and instead you had stock there the CAM didn't know about. This sounds like a logical explanation for what happened. Just because it reversed direction (+Y toward -Y) doesn't mean the cut would have been climb if the stock didn't exist there.

CAM is what limits the usefulness of CNC in the home shop. When I got into it I played with the free stuff out there and made a few parts with dxf->gcode programs that existed in 2006 or so. I quickly realized that if I wanted to make anything 3D I need a real CAM software that was going to cost 1000-4000USD. I ended up with VisualMill for 750USD or so. It works, and if you figure out it's quirks you can trick it into doing exactly what you want, but it doesn't do anything fancy. I added a 4axis and looked at CAM again this year. Anything that does continuous 4th starts at 4000USD.

 

[laurent_parti]

OK... So the slomo video threw me. Your actually going too fast, way too fast. :fan:

Your radial WOC is far too much (on that first step down in the parallel lace operation anyway) I don't know what CAM you use but in a lace operation you should be able to define entry parameters such as helical, 3d path or 2d path options for this purpose. On the pass to go down to the next level you can specify how many steps to take to get to depth.

If you don't have these options you can always machine away material for clearance.

I've really come to dislike parallel operations over the years. Try a spiral path, choose a start point in the middle of the part. You'll never engage more of the tool than you want.

Here's what I get when I put your parameters in:

Thanks JW for your answer. My CAM soft is not able to do this 3D milling in other way than parallel. I share your though regarding it.
Many Thanks for your parameters inputs, I will make some testings this week-end and maybe a new video !

 

[laurent_parti]

I try to run .001-.002" per tooth and I often run ~15,000 RPM. Depth of cut and stepover are somewhat limited by the rigidity of the machine. I usually run 75% stepover, to avoid problems with full width cuts. A very good (expensive commercial grade) CAM would allow me to run the parameters I'd really like, but if I had the money I'd be running a Hass Minimill or similar instead of my frankenmill.

A slotting (full width) pass is always conventional, think about it.

In the video, the aluminum overheated, clogged the flutes, stopped cutting, and broke. With some lubricant it may have made the cut. Depends on the grade and hardness of aluminum and the cutter type.

Have you checked tool runout when installed in the spindle? Too much runout effectively makes your two flute a single flute and the feedrates will be wrong which kills the cutter. 0.5mm DOC at 400mm/min is about all I could do with my old spindle. Another issue is plunge feed rate, this used to kill me a long time ago. If you attempt to plunge at the full feed rate it will instantly clog the cutter in AL.

Did you define your stock properly in your CAM? Maybe it thought your stock was equal to the extents of the part, which means it thought it would be making a small radial cut and instead you had stock there the CAM didn't know about. This sounds like a logical explanation for what happened. Just because it reversed direction (+Y toward -Y) doesn't mean the cut would have been climb if the stock didn't exist there.

CAM is what limits the usefulness of CNC in the home shop. When I got into it I played with the free stuff out there and made a few parts with dxf->gcode programs that existed in 2006 or so. I quickly realized that if I wanted to make anything 3D I need a real CAM software that was going to cost 1000-4000USD. I ended up with VisualMill for 750USD or so. It works, and if you figure out it's quirks you can trick it into doing exactly what you want, but it doesn't do anything fancy. I added a 4axis and looked at CAM again this year. Anything that does continuous 4th starts at 4000USD.

Thanks dieselpilot for your inputs. Cooling and lubricant have to be managed with high care because my CNC is made from plywood ( lol ).

Agree with the plunge speed, I discovered that my CAM soft manage speeds in the same value for all the axis (damn). So I had to modify "by hand" the Gcode and maybe I forgot a line to reduce speed during plunge !
I did not check the runout and the tool is now broken but it is a great thing to do on the set-up check-list. Will add it.
Regarding the CAM soft, I guess I will have to make a step further like you did !

Thanks again

 

[dman]

i agree with the heat, the chip load is .002 per tooth and that might be a lot for such a small diameter, it should be doable but you may want to cut it down by half. the heat is because you have a wooden machine. i once made a complicated aluminum bracket and i had to do a compound angle. i used a piece of thick piece of lexan to fixture the part onto as something i could cut into without increasing the loads or causing chatter. well the part cut fine at first but the heat built up and started gumming up the endmill which had ample chip clearance and i noticed the metal was extremely hot. the plastic kept the heat in despite me trying cutting oil. you don't really realize how much heat the table on a mill sucks out untill you have a heat problem on a non metal table.

try to use compressed air, or a cold air vortex tube if you can. i've also heard of using alcohol as a coolant while cutting aluminum but never tried it. you should make sure the cutter is sharp and you may find climb milling to work better if you get the chip loads right.

vortex tube, incase you are not familiar;

www.exair.com/en-US/Primary Navigat...Pages/Vortex Tubes and Spot Cooling Home.aspx

 

[Wizard69]

i agree with the heat, the chip load is .002 per tooth and that might be a lot for such a small diameter, it should be doable but you may want to cut it down by half. the heat is because you have a wooden machine. i once made a complicated aluminum bracket and i had to do a compound angle. i used a piece of thick piece of lexan to fixture the part onto as something i could cut into without increasing the loads or causing chatter. well the part cut fine at first but the heat built up and started gumming up the endmill which had ample chip clearance and i noticed the metal was extremely hot. the plastic kept the heat in despite me trying cutting oil. you don't really realize how much heat the table on a mill sucks out untill you have a heat problem on a non metal table.

try to use compressed air, or a cold air vortex tube if you can. i've also heard of using alcohol as a coolant while cutting aluminum but never tried it. you should make sure the cutter is sharp and you may find climb milling to work better if you get the chip loads right.

vortex tube, incase you are not familiar;

www.exair.com/en-US/Primary%20Navigation/Products/Vortex%20Tubes%20and%20Spot%20Cooling/Pages/Vortex%20Tubes%20and%20Spot%20Cooling%20Home.aspx

I'd try other things before alcohol, the idea of a flash fire just isn't appealing.

On another point WD40 works amazingly well on aluminum. A second point is check you tooling closely to make sure it is even recommended for Aluminum. This is especially the case for coated tools where some coatings have an affinity for aluminum. If uncoated or coated with something compatible with aluminum make sure you are using a minimal number of flutes with fast spirals. In some cases a single flute cutter can be justified for aluminum and you really should think hard about using more than two flute cutters.

 

[laurent_parti]

i agree with the heat, the chip load is .002 per tooth and that might be a lot for such a small diameter, it should be doable but you may want to cut it down by half. the heat is because you have a wooden machine. i once made a complicated aluminum bracket and i had to do a compound angle. i used a piece of thick piece of lexan to fixture the part onto as something i could cut into without increasing the loads or causing chatter. well the part cut fine at first but the heat built up and started gumming up the endmill which had ample chip clearance and i noticed the metal was extremely hot. the plastic kept the heat in despite me trying cutting oil. you don't really realize how much heat the table on a mill sucks out untill you have a heat problem on a non metal table.

try to use compressed air, or a cold air vortex tube if you can. i've also heard of using alcohol as a coolant while cutting aluminum but never tried it. you should make sure the cutter is sharp and you may find climb milling to work better if you get the chip loads right.

vortex tube, incase you are not familiar;

www.exair.com/en-US/Primary%20Navigation/Products/Vortex%20Tubes%20and%20Spot%20Cooling/Pages/Vortex%20Tubes%20and%20Spot%20Cooling%20Home.aspx

Thanks dman for informations. I know the vortex tube and it is great but just eat huge ton of air lol. I use a Koolmist nose and the temperature looks like pretty good but I do not use coolant.
Alcohol is adviced sometimes but I will be afraid of a fire. I heard it is use with 50% water to cut acrylic. The cutter was supposed to be new but I did not check if it was sharp. Next time I will.

 

[laurent_parti]

Thanks Wizard69.

I share the idea of fire. WD40 is a great idea, I will definetly try it.
The other point link to the compatibility of the coating is great to consider. I do not know if this end mill has one and if it is ok for aluminium.

Will check with the supplier. Thanks.