Hi,

On saturday I finished the Z axis so that my BF-16 mini mill was fullly operational. I started to do some test cuts and I had mixed results. When I do a contour cut through solid aluminum taking about 1mm cuts, I get a lot of tool marks on the sides of the shape. I thought that this was chatter, but I have a collet chuck with bison collets. So I proceeded to find the problem. I locked the y axis jib so that it could not move as well as the z axis while I was doing straight cuts on the x-axis. Still the same results. Then it looked like the chips were causing the problems so I cut a groove about 1cm wide and proceeded to cut along one of the walls.

This is what I found. Using a 4mm solid carbide 2 flute tool bit and taking a stepover of 2mm and stepdown of 1mm on one of the walls. The tools is spinning clockwise, and if I move from right to left I get a perfect cut no marks on the wall and I do not touch the tool chips that are on the wall prior to the cut. If I move from left to right, then I start to get all of those tool marks and when I go back to the left it the next cut down is perfect.

Now, is this a problem with the tool that I am using? Or something else? Lets discuss.

Thanks

Sebastian

Climb milling is the usual preferred method, that would be your CW rotation moving from right to left, what you are seeing is caused from re-cutting the chips. Because you do not always have complete control to climb mill or conventional mill it will help to keep the chips blown out or better yet flooded out if you can incorporate that into your system. You might also try a higher helix cutter designed for aluminum, they move the chips up and out of the way quicker.
Here is one link for them.

http://www.lscarbide.com/products.asp?cat=32

Climb milling is the best way to go IF your machine has little or no backlash. Backlash will show up as chatter in your material when climb milling.
Climb milling is as if the endmill is pulling the material into the endmill whereas conventional milling is when you are feeding the material into the oncoming cutting edge of the endmill.
Colin

I'm no expert but here's my 2 cents worth:

I'm not sure a 2 fluted slot mill is the best for this aplication, also you don't say anything about spindle rpm or feed rate. A photo of the offending tool marks might help in Identifying the problem. Also what quality of carbide cutter are you using and how sharp is it. How uniform are the tool marks.

With climb milling, in your particular senario, the cutter tooth is approaching the face of the workpiece at 90 degrees. Which is the kindest for the cutter if it is not as sharp as it should be. With conventional milling the tooth has a very narrow approach angle so it has to be forced into the workpiece which might cause problems for a blunt cutter with regard to flexing under load.

Regards
Phil

Hi,

On saturday I finished the Z axis so that my BF-16 mini mill was fullly operational. I started to do some test cuts and I had mixed results. When I do a contour cut through solid aluminum taking about 1mm cuts, I get a lot of tool marks on the sides of the shape. I thought that this was chatter, but I have a collet chuck with bison collets. So I proceeded to find the problem. I locked the y axis jib so that it could not move as well as the z axis while I was doing straight cuts on the x-axis. Still the same results. Then it looked like the chips were causing the problems so I cut a groove about 1cm wide and proceeded to cut along one of the walls.

This is what I found. Using a 4mm solid carbide 2 flute tool bit and taking a stepover of 2mm and stepdown of 1mm on one of the walls. The tools is spinning clockwise, and if I move from right to left I get a perfect cut no marks on the wall and I do not touch the tool chips that are on the wall prior to the cut. If I move from left to right, then I start to get all of those tool marks and when I go back to the left it the next cut down is perfect.

Now, is this a problem with the tool that I am using? Or something else? Lets discuss.

Thanks

Sebastian

tt_raptor_90,

As mensioned before Climb Milling with light cuts for finishing and Convensional for Roughing. Try 3 flute end mills. Don't cut on the end of the end mill and the side at the same time. This can cause higher cutting forces and put strain on your collet.
Are you using any type of coolant? Last but not least by far, you mension using a Bison collet. Bison collets aren't that great, they tend to have a lot of runout. Try a different brand of collet like Hardinge, ETM (Iscaar), or others. Collets again aren't as rigid as solid tool holders. What taper does the machine spindle have? (Not familiar with the specific brand of mill)

Good luck, you have lots of things to try in this Thread.

Hope you find your problem.

tobyaxis :cheers:

Hey,

So here is the update. I am running a Quantum Vario BF-16 benchtop mill with MT2 spindle and 3000rpm spindle speed when I am cutting. I will try to post some pics tonight about the problems.

The feed rate that I use is 300mm a min on x&y and 400mm a min on Z. The cutter was the best quality of solid carbide from a store that just sells cutting tools and Hardinge machinery. When I do the cutting, I use a vacuum to remove the chips.

Last night I did some more cuts and I am confused. First cut was a pocket circle in aluminum. I left 0.2mm for the finish cut, and I left 0.5mm for the final pass of the rought pocket. Now, when it does the rought cut, the machine move clockwise. When the pocket was done and a 0.5mm ring was left, it did a perfect cut with no marks on the wall. It did this for the whole pocket then it started the finish cut. For the finish cut it moves counter clockwise and the wall was perfect again. Same for a gear that had all of the material removed around it.

So could the problem be that this tool is not designed to do single pass contour cuts where is has aluminum walls on both sides?

Also, the marks on the pieces are not uniform at all. At the top, it has a smooth pass, and the farther you go down the worse they get. At first they are spread out little scratch marks and then they start to bunch together.

Thanks

Sebastian

If I understand you right you tightened down the Y axis gib and are contouring in z and x axis. This would be better referred to as the G18 plane. The endmill you are using is a centercutting slot mill solid carbide. This tool has only one effective cutting edge on the Z axis that crosses over cutter centerline and you are plunging with it. Your feetrate is excessive. Feedrate is calculated by number of effective cutting edges times chip thickness times RPM. Keep the chip thickness (ipt or mmpt) to about .0008 imperial or .015 millimeters . If you cant slow the feedrate try a cutter with more cutting edges and clear the path for the center of the cutter in Z for the plunge.
Best of luck.. Drum.

Another 2 cents worth:

Your feed rates of 300 to 400 mm is way to high. With 3000 rpm and a 2 flute carbide end mill a VMC feed rate would only be 100 mm/min.With a hobby machine you should probably run 2/3 to 1/2 of this so a feed rate of 50 to 70 mm/min sounds about right.

I'm still a bit confused as to whether you are cutting a slot or a pocket. A pocket is bigger than the width of the cutter a slot has a width equal to the cutter diameter. Slots are traditionally difficult to achieve an accurate slot with good surface finish. If you need a "good" slot then rough it as a slot and finish it as a pocket.

Photos will help a lot.
Regards
Phil

Hey,

So here is the update. I am running a Quantum Vario BF-16 benchtop mill with MT2 spindle and 3000rpm spindle speed when I am cutting. I will try to post some pics tonight about the problems.

The feed rate that I use is 300mm a min on x&y and 400mm a min on Z. The cutter was the best quality of solid carbide from a store that just sells cutting tools and Hardinge machinery. When I do the cutting, I use a vacuum to remove the chips.

Last night I did some more cuts and I am confused. First cut was a pocket circle in aluminum. I left 0.2mm for the finish cut, and I left 0.5mm for the final pass of the rought pocket. Now, when it does the rought cut, the machine move clockwise. When the pocket was done and a 0.5mm ring was left, it did a perfect cut with no marks on the wall. It did this for the whole pocket then it started the finish cut. For the finish cut it moves counter clockwise and the wall was perfect again. Same for a gear that had all of the material removed around it.

So could the problem be that this tool is not designed to do single pass contour cuts where is has aluminum walls on both sides?

Also, the marks on the pieces are not uniform at all. At the top, it has a smooth pass, and the farther you go down the worse they get. At first they are spread out little scratch marks and then they start to bunch together.

Thanks

Sebastian

Hi,

So the problem only occurs if I try to do a single contour cut. If I make a contour cut/pocket cut and leave 0-1mm of excess material, than the finish cut is perfect. So should I just use this method or have other people been able to do single pass finish cuts?

For the feed rates I run about a 60% of toolbit stepover and 0.5 mm stepdown. With these feedrates I will get a mirror finish if I do a roughing pass and a finish pass. 50-60mm a min seems quite slow but I am new at this and would like to get an opinion based on the values that I provided above. With 300mm a min feedrate on x and y and a 60% toolbit stepover is this too fast?

Thanks for the help,

Sebastian

Per the Machinery's Handbook: material=6061, mill dia=.250, feed / tooth=.002, SFM for carbide=620.

Given your 4mm 2 flute end mill lets assume .001" feed/tooth.

Per Cimco Feed/Speed calculator: Tool Data=.156" dia mill,2 flutes,.001 feed/tooth, 620SFM.
Result: RPM=15181, feedrate=30 IPM.

Seeing as you can only spin 3000 RPM an equation is in order.

30 _____ X
----- = --------
15181 __ 3000

Solve for X.
30X3000=90000
90000/15181=5.93"/minute

5.93/.0393701=150.6mm/minute feedrate

Now lets see how good the book and software are???

Ken

Exactly Ken,

And of course this is only what the cutter is good for (ballpark). What the machine can handle and still produce a good finish is another matter. MHB is about commercial operations with commercial machines with appropriate rigidity. Reduce the forces to allow for a hobby machine and you are down to something like 50 to 75 mm/min.

At the end of the day, for a given spindle speed, if the feed rate you are using produces a bad finish you have two main options to improve it. Reduce the feed rate or improve the rigidity.

Understanding together with experimentation is the key for the hobbyist.

Regards
Phil

Per the Machinery's Handbook: material=6061, mill dia=.250, feed / tooth=.002, SFM for carbide=620.

Given your 4mm 2 flute end mill lets assume .001" feed/tooth.

Per Cimco Feed/Speed calculator: Tool Data=.156" dia mill,2 flutes,.001 feed/tooth, 620SFM.
Result: RPM=15181, feedrate=30 IPM.

Seeing as you can only spin 3000 RPM an equation is in order.

30 _____ X
----- = --------
15181 __ 3000

Solve for X.
30X3000=90000
90000/15181=5.93"/minute

5.93/.0393701=150.6mm/minute feedrate

Now lets see how good the book and software are???

Ken

Ken, those feeds and speeds seem way too high. The MHB is a reference for standard starting points. It doesn't give formulas for machine or part rigidity.
TT_raptor_90 will have to experiment with his machine to see what it will handle.
A CAT50 spindle VMC machine will usually cut aluminum 6061-T6 at 6,000 RPM at around 150 IPM (tool 3/4 emill duramill .375 doc and full width 3 flute) on a solid block measuring 6x6x6 in a Kurt Vise. A machine with more RPM range same CAT50 Spdl will do it even faster. When a tool squeels turn the RPM down so it can equil it's self out with the feed rate. Not the same case with a mini milling machine. ;)

tobyaxis