[Jig Maker]

I am milling the patterns you see in the pictures. I am making a rough pass with a .5" 2 flute straight bit at 4"/m, then a finish pass with the same bit at 10"/m.

Retool with a 2 flute 10° dovetail bit .625 width to get the profile needed below the plate. Dry cutting.

My questions . . . . .

• Would the Amana O Flute bit be a better option than the 2 flute straight bit I am using?
• Would wet cutting allow a significantly higher feed rate?
• Based on this brief description can anyone offer some way I can get longer life from the bits?

You can see the cross section below, and where the k-shape cross section in the center is where the bits labor obviously, so that's the main reason for the slow feed rates since I don;t want to sit there and manually slow it down through that section.



Here you can see the dovetail profiles being cut.



I have extensive fabrication/woodworking/electrical/JOAT experience but I am a brand new newbie when it comes to CNC. So anyone who may offer some suggestions please keep it as non-technical terms as possible. Thanks. Kevin.


.

[Jig Maker]

I also meant to ask what could be causing the dovetail bit to leave so much molten metal (slag?) or whatever it's called. It's like pulling teeth to get it off. The straight bit I'm using leaves a nice finish on the top . . . . .




But the dovetail bit leaves all this garbage behind . . . . . .




. . . and I slowed the feed down to .5/m but it didn't make any difference.

I will probably answer my own question and catch hell for it too, but the straight bit is Italian and the dovetail is Chinee. I guess that must be the difference. Can carbide be so poor quality as to be more like HSS?

I will get a Diablo bit tomorrow an try it but the POJ chinee dovetail bit was the only one I have with the profile I needed.

[78nova]

My first thought would be that you are using some very weak tools.

The " Slag " you mentioned appears to be uncut material.

This will happen when a cutter is dull or ground wrong.

The tool is rubbing off most of the material, rolling it up into the slag as you called it. We call these welded chips. The heat being generated by the cutter not working correctly, is rolling up and rubbing off the material.

A few different things could be wrong.

Dull tool, incorrect tool grind / relief.

Wrong stlye cutter for application / material.

Yes, there is carbide that will not cut as good as others.

Yes, a good cutting oil will improve tool life over running dry.

Dry cutting has it's place but your situation / material is not one of them.

I am not familar with your material and if it is anodized as you stated that will help dull up a cutter quicker than normal.

How stable is your work piece? Could you use a bigger first tool?

What RPM is used on each tool.

Is your abbreviation .5/m, mean 1/2" ipm ( inch per minute )

What are your cut dimensions?

Profile radius? Width of cut? Depth of cut? Length of the 10 degree cut and corner radius on both tools?

Kenny

[Jig Maker]

Kenny,

Thanks for your thorough reply. I will try to answer your questions accurately as I can.

How stable is your work piece? Could you use a bigger first tool?

It seems very stable but I do need to devise a better hold-down. I could use a larger tool but I can't find one with the profile I need.


What RPM is used on each tool.

When I first made this post, I had the router set to 16,500. I had thought it was set to 23,000 but wasn't. Now with the higher RPM's the cuts have improved a great deal. No more molten chips.


Is your abbreviation .5/m, mean 1/2" ipm ( inch per minute )

Yes it is 1/2 ipm. I thought machinists used decimals. I'm used to fractions so that's good news.


What are your cut dimensions?

I make a rough pass with the 1/2" bit, and it cuts through the profile as you see for 3 3/8" and right before it reaches the other side of the top plate, it turns making a radius of 5/8" and when it comes back out there is ~ 3/4" width in the slot, less whatever the finish pass takes which I think is a 64th inch.

After those two passes, then the retooling with the dovetail bit. The dovetail cut is working out very well now. I bought a better bit and slowed the feed rate a little more. It's making beautiful cuts. I would like to speed up the feed rate though so I'll have to research how to add an oil system. I dread that though. It's gonna play hell on slowing things down. I'll have to weigh whether the slower feed rate may be faster than all the clean up that will have to take place both the jigs and the router. Not to mention the vacuum is bound to start collecting oil. I hate to even think of what all that might add. Could very well be better to just cut dry?


Profile radius? Width of cut? Depth of cut? Length of the 10 degree cut and corner radius on both tools?



I think I answered most of those above, but I really don't know what a corner radius is. Thanks again for your answers.

[78nova]

Sounds like you have had some better luck with your tooling.

After reading your comments about how introducing oil would be a headache, I remembered there are alternative ways to help cool the tool.

Take a look at this site.
http://www.vortexair.biz/Cooling/Col...oldairgun.html

Over in our manual area these are used at times and they do seem to work out OK. I have never used one since my machine is enclosed so I am able to run oil with no problems like you would encounter.

Machinist do use decimals mostly, I used a fraction to ensure we both knew what the amount was we were both referring to.

A corner radius is the radius that is on the corner of the cutting flute.

A coating on your tools like TICN or TAILN might help with your tool life also.

If it is at all a problem milling over in the corner where your 5/8" profile radius is you could take a 1/2" drill or smaller to create a pilot hole and drill through down onto the center of this profile. You could then also take a 5/8" drill and follow that to drill through.

This would then allow your 1/2" end mill to work less in the corner and already have your 5/8" profile radius formed. You could also then bump up your tool to a .625 diameter to give you a little more rigidity in your tool.

This might lead to being able to increase your feed rates some. Just a thought.

This of course would also have to take into consideration what your slot width and profile radius tolerance is. The more tolerance, the more room to play around some in searching for improvements to a process.

Your part configuration is somewhat unique but when we can, we will either drill out the corners in some of the pockets we do so the tool does not chatter by working too hard in the corners. We also at times will take the end mill and make it run a drill cycle to bore out these corners to form a nice clean profile. Then when we mill through this area so we can maintain our feedrate and not worry about the tool chattering the finish profile.

You mentioned working on a better hold down. What if you added a top plate to the part that was in the same basic top shape & slot configuration as your part but with the slots about 1" to 1-1/8" wide to provide tool clearance and was the same length as your part. This top plate could be held down with the two end clamps you are now using.

I am not sure what your part edge thickness is but even if the top plate was 1/4" to 5/16" thick and you were able to add a lead backing to it, I think this would possibly help provide some improvement to your holding the part while providing a deadening effect from the top plate lined with lead by reducing vibrations caused by your cutting tools and your " K " shaped part cuts.

Wheh!

Just thought I would throw out a few ideas at you to see if it might help you some if any.

Good luck. :wave:

Kenny