[cmelo]

I'm sure to leave something out that someone will ask me. This is also my first post to this forum so hopefully it's in the right place.

I'm making a .5" diameter, slightly over 4" deep flat bottom hole in 6061 aluminum. I have a Harvey Tool 3/8" relieved shank stub flute square endmill that has a reach of 4-9/16" that I can't quite get a handle on speeds and feeds. I'm also open to what other tools might do it better. The only kicker is I am drilling a 3/8" hole first that is also about 4" deep that has a center point very close to the center of the .5" hole. Making it difficult to drill both holes out. So I had to take a pick as to which one I'll drill and which one I'll have to mill out after. The bigger hole seems like the better choice of the two.

I have measured run out on the end mill. At the top it is less than .0005" but I only have a .0005" indicator right now. Towards the bottom, near the flutes I'm getting more like .001" and I have tried rotating the tool and collet and get the same result. I ordered a new collet for a better a TG collet holder we have but it won't be here until tomorrow. I'm sure it would help to get the run out down under .0005" at the bottom as well.

I run the tool at 10,000RPM and rough out the hole at 33IPM using a helical ramp. By helical ramp I mean the code is outputting a circular interpolation that also uses the Z. This surface finish is OK, atleast for a roughing pass. For a finishing pass I've tried what seems like everything. Different RPMs(slow and fast) as well as feeds that vary. Very rarely I feel that I have encountered an endmill that can't be run at a fast spindle speed and slow feed in 6061 for a good surface finish. This tool however just can't handle it. Even at 10,000RPM and feed of 1ipm and radial load of .005" the chatter is unbelievable. I've also tried loading it better with 10,000rpm, a feed of 40IPM and a radial load of .036" as per recommendations. Still terrible finish and chatter.

We have an Iscar multimaster with a 3/8" shank and a 1/2" ball insert that is able to easily give me a great surface finish at similar speeds and feeds. This tool is also 4+" long. I'm not quite sure what I'm doing wrong or if there is a different approach or tool/tools I should be using instead. When you start getting into these long end mills things get pretty hairy. Although, I've machined stainless with .062" 12X diameter end mills with good success. This big 3/8 cutter however is giving me nothing but grief. I know Harvey makes a great tool so I don't know where to point.

To double check speeds and feeds I've put the numbers into the FSWizard calculator on CNC Tricks Home and with a feed of 33ipm, .5" DOC and .036" radial cut it tells me that I should see .005" of deflection! These are feeds that I'm testing directly from Harvey. Typically when I use this calculator I would shoot for deflection of .0005" or less. However, I was told I was not properly loading the tool with feeds as low as I was using this way. It does seem to react fairly well to the higher feeds, especially on the helical ramp down.

It may just be that I cannot get this tool to any side milling at all. That's what it seems like. The ramp down it sounds pretty good. Surface finish isn't what I need it to be but not the totally messed up finish I get from trying to take a finish pass. I may also need to try and track down this .001" of run out which can be a lot for this length tool. I feel as though I've tried every speed/feed combo possible. If I choose to drill it out and follow with an end mill to get a flat bottom that will work but then I'm left milling out a 3/8" round "Keyway" which would mean using a 1/4" endmill of similar length.

If anyone managed to read all that and has any input I'll be eager to hear it!

[stucapco]

wow, get it close then send in a finishing bore canned cycle. I use a lathe thread bar with modified inserts in my VMC's. Get the pressure off the finishing pass. I'm amazed at the results your now getting. Interesting...

I should add these are helical interpolations, any size, depths limited to the tool reach. My point here is to get the pressure off the final finish pass.

Hope this helps.

[cmelo]

wow, get it close then send in a finishing bore canned cycle. I use a lathe thread bar with modified inserts in my VMC's. Get the pressure off the finishing pass. I'm amazed at the results your now getting. Interesting...

That was my other thought. Get a boring head and carbide boring bar and use a boring cycle. Any reason you use threading inserts? I would think I wouldn't want that since I'm looking to come to a square shoulder(some radius would be fine). I was worried that the diameter boring bar I would need to fit in a .5" hole may also not be very rigid.

Thanks!!

[stucapco]

Well, old tired threading inserts I have plenty. Grind them into something usable. Make the the reach or size work in your favor. I wasn't thinking boring head but ok that gets the pressure off the finishing pass and will tend to be more accurate than a helical interpolation as we're not depending on the machines axial movement tolerances. If it works, IT WORKS! Plain and simple, might cost you a little time to work it out but if the end result is within tolerance, I'm all for it.

Luck.

[MetalCarpenter]

Is this fanuc control? Give me the print dimensions of the hole and list the tools you have.i believe I can help. ..

[cmelo]

Is this fanuc control? Give me the print dimensions of the hole and list the tools you have.i believe I can help. ..

It is a 2008 HAAS Mini Mill. The dimensions for just the hole really is just .500" to a 4" depth. The only tools I have right now to make the cut is the Harvey tool I listed above and a 1/2" diameter HSS end mill that is just over 4" long. I have tried peck drilling with the 1/2" end mill but it results in an oversized hole. I plan on buying a flat insert to use on the Iscar Multimaster to try. Maybe I have a lathe boring bar I can grab before I go to work tomorrow to try and test out as well.

I'd love to hear your thoughts.

[stucapco]

Drill it a 64th under and ream it? Quick, easy, cheap. Downside, depending on speeds and feeds it may wander from perpendicularity. Boring is best however you may not need this accuracy compared to effort involved.

Luck.

[MetalCarpenter]

It is a 2008 HAAS Mini Mill. The dimensions for just the hole really is just .500" to a 4" depth. The only tools I have right now to make the cut is the Harvey tool I listed above and a 1/2" diameter HSS end mill that is just over 4" long. I have tried peck drilling with the 1/2" end mill but it results in an oversized hole. I plan on buying a flat insert to use on the Iscar Multimaster to try. Maybe I have a lathe boring bar I can grab before I go to work tomorrow to try and test out as well.

I'd love to hear your thoughts.

Is the length of cut on the end mill just over 4 as well
??

[cmelo]

Drill it a 64th under and ream it? Quick, easy, cheap. Downside, depending on speeds and feeds it may wander from perpendicularity. Boring is best however you may not need this accuracy compared to effort involved.

Luck.

I could drill it. Like I think I mentioned however it "passes through" a 3/8" hole as well. That's not a good description but a 3/8" hole overlaps the .5" hole so I cannot drill both holes since whatever hole I drill first will cause the second drill to wander into the first hole. It would seem to me more ideal to drill the smaller of the two holes and mill/bore the second bigger hole.

Is the length of cut on the end mill just over 4 as well
??

The LOC on the 1/2" endmill is just over 4". The 3/8" endmill the LOC is 9/16" with a relieved shank.

[stucapco]

After rereading this post, is flipping the part and hitting it from the back an option? I admit I am tired right now and don't completely see it. We're boring a larger hole through a smaller hole slightly off center of the original hole? A rough sketch would be helpful. I believe we're on the same page just not connecting through words. Forgive me here, I want to help. A visual (print, drawing) would clear it up for me.

[cmelo]

After rereading this post, is flipping the part and hitting it from the back an option? I admit I am tired right now and don't completely see it. We're boring a larger hole through a smaller hole slightly off center of the original hole? A rough sketch would be helpful. I believe we're on the same page just not connecting through words. Forgive me here, I want to help. A visual (print, drawing) would clear it up for me.

I can't post a full drawing but I could post up the basic feature. It's a blind hole so it cannot be flipped and machined from the other side.

[cmelo]

Attachment 271228

I made the worlds simplest drawing of a representation of the feature I'm making. I left out a lot from the actual part and this only took me a minute so if it's still confusing that's why. I think it's better than trying to describe it though.

Thanks for all the help so far guys

[MetalCarpenter]

Attachment 271228

I made the worlds simplest drawing of a representation of the feature I'm making. I left out a lot from the actual part and this only took me a minute so if it's still confusing that's why. I think it's better than trying to describe it though.

Thanks for all the help so far guys

drill a 375 hole to z-3.990 w a twist drill using a spot drill first.

position the first x position to -.05 from where center of.375 hole is to have room to turn on cutter comp for .500 hole...y position center of the .375 hole.we will use. 375 hole as a clearance hole to feed down in to do the .500 partial hole

T02 IS THE .375 END MILL .5625 LOL REDUCED SHANK

T02 m06
G0 G90 G54 x_ y_ S2000 M03
g43 h02 z1.0 M08 (air blast preferred)(I would hold air nozzle and blow it out while running w no coolant)
Z.1
G01 G41 D02 F20. X_ (to center of .375 hole)(comp on)
g01 z0 f10.
M97 P1000 L77 (jumps to line n1000 & repeat subroutine 77 times)
G90
G99 G83 R-3.865 Z-3.998 Q.002 F1.2 (peck hole to take out drill tip)
G0 G80 Z-3.865
G01 Z--3.995 F3.0
G01 Z-4.0 F.75
S2500(finish rpm)
G01 G91 X or Y F5.0( incremental distance to center of .500 hole just like before)
G13 I0 K.0625 Q.002 F20. (Moving a Lil faster here don't worry)
(now to finish hole going up in steps a lil less than the loc of the endmill)
G90
G01 Z-3.5
G91 G13 I.06 K.0625 Q.0008
G90 G01 Z-3.0
G91 G13 I.06 K.0625 Q.0008
G90 G01 Z-2.5
G91 G13 I.06 K.0625 Q.0008
G90 G01 Z-2.0
G91 G13 I.06 K.0625 Q.0008
G90 G01 Z- 1.5
G91 G13 I.06 K.0625 Q.0008
G90 G01 Z-1.0
G91 G13 I.06 K.0625 Q.0008
G90 G01 Z- .5
G91 G13 I.06 K.0625 Q.0008
G0 G90 Z1.0 M9
G1 G40 X or Y (move to turn off cutter comp)
G28 G91 Z0
G28 G91 Y0
M30






N1000
g91 g01 z-.050 f4.0
g01 x or y distance to center of .500 hole F10.(this is incremental)
G13 I0 K.06 Q.005 F10.
g01 x or y F4.0 ( move incremental back to previous position (incremental in x or y depends which way your setup)
M99




Make sure to have the N1000 thru m99 after the M30 and no other n1000 blocks besides that one in your program


let me know how it works.

[MetalCarpenter]

Attachment 271228

I made the worlds simplest drawing of a representation of the feature I'm making. I left out a lot from the actual part and this only took me a minute so if it's still confusing that's why. I think it's better than trying to describe it though.

Thanks for all the help so far guys

I really believe the tool path is what will make this successful.not preaching to choir or underestimating you but I believe line by line programming on this application is best to get desired tolerance results

[stucapco]

Get the pressure off the secondary oblong machining. It will produce better/reliable results. Period. Your "elbow deep", on the edge. Free cuts. Find what works for you and i'm guessing here (not guessing)... DO THAT!

This is so much fun!

Luck.

[cmelo]

drill a 375 hole to z-3.990 w a twist drill using a spot drill first.

position the first x position to -.05 from where center of.375 hole is to have room to turn on cutter comp for .500 hole...y position center of the .375 hole.we will use. 375 hole as a clearance hole to feed down in to do the .500 partial hole

T02 IS THE .375 END MILL .5625 LOL REDUCED SHANK

T02 m06
G0 G90 G54 x_ y_ S2000 M03
g43 h02 z1.0 M08 (air blast preferred)(I would hold air nozzle and blow it out while running w no coolant)
Z.1
G01 G41 D02 F20. X_ (to center of .375 hole)(comp on)
g01 z0 f10.
M97 P1000 L77 (jumps to line n1000 & repeat subroutine 77 times)
G90
G99 G83 R-3.865 Z-3.998 Q.002 F1.2 (peck hole to take out drill tip)
G0 G80 Z-3.865
G01 Z--3.995 F3.0
G01 Z-4.0 F.75
S2500(finish rpm)
G01 G91 X or Y F5.0( incremental distance to center of .500 hole just like before)
G13 I0 K.0625 Q.002 F20. (Moving a Lil faster here don't worry)
(now to finish hole going up in steps a lil less than the loc of the endmill)
G90
G01 Z-3.5
G91 G13 I.06 K.0625 Q.0008
G90 G01 Z-3.0
G91 G13 I.06 K.0625 Q.0008
G90 G01 Z-2.5
G91 G13 I.06 K.0625 Q.0008
G90 G01 Z-2.0
G91 G13 I.06 K.0625 Q.0008
G90 G01 Z- 1.5
G91 G13 I.06 K.0625 Q.0008
G90 G01 Z-1.0
G91 G13 I.06 K.0625 Q.0008
G90 G01 Z- .5
G91 G13 I.06 K.0625 Q.0008
G0 G90 Z1.0 M9
G1 G40 X or Y (move to turn off cutter comp)
G28 G91 Z0
G28 G91 Y0
M30






N1000
g91 g01 z-.050 f4.0
g01 x or y distance to center of .500 hole F10.(this is incremental)
G13 I0 K.06 Q.005 F10.
g01 x or y F4.0 ( move incremental back to previous position (incremental in x or y depends which way your setup)
M99




Make sure to have the N1000 thru m99 after the M30 and no other n1000 blocks besides that one in your program


let me know how it works.

I really believe the tool path is what will make this successful.not preaching to choir or underestimating you but I believe line by line programming on this application is best to get desired tolerance results

We have what looks like a similar approach in how we would go about it. You however are much better at hand written Gcode. I've never tried a G97. I feel bad, the drawing I posted wasn't a direct representation of the part. So the code you so generously provided would not work. I would be interested in some reasoning behind what you did. Like your speeds and feeds. Why such a slow spindle speed? I've tried slower speeds and I suppose at slower speeds you can more appropriately run it at slower feeds. I've tried various different combinations but Harvey swears by running it at the full 10,000rpm of our machine.

Get the pressure off the secondary oblong machining. It will produce better/reliable results. Period. Your "elbow deep", on the edge. Free cuts. Find what works for you and i'm guessing here (not guessing)... DO THAT!

This is so much fun!

Luck.

Not sure I understand


As a bit of an update. I rechecked run out on the Harvey tool. I bought a brand new Lyndex collet for a Lyndex TG holder we have, cleaned everything out and chucked it in the mill. With my .0005" indicator I measure about .0005" at the top but a whopping .0025" towards the bottom. The iscar Multimaster we have has .0005" tops at the same distance away(as far I can tell with my indicator, could be less). I ordered a square end mill for the multimaster small enough to reach into a .5" bore and have room to do some circular interpolation. If this tool works I think that I have found my culprit. If not I may try the boring bar.

[stucapco]

So, I'm seeing a .0025 out if square relative to the table, machine or fixture. .0005 is acceptable as far as rapid repeatability. Is this an acceptable tolerance? Again, now that I see it better, get it close. free cut (by this I mean no pressure one way or the other) on the tool. Lets clarify, in the case of an endmill we are always pushing on it one way or another (damn cutter deflection over this distance can be a bear). Now lets assume the boring bar only touches a small cutting percentage (clean up). It will have the same stress on it top of the part as bottom (not true, we're still dealing with the deflection from the previous cutter). However much closer and far more likely to be true (the machines perpendicularity to the table, fixture. etc) to the goal expected. I know that sounds like double talk. What would happen if we ran this cycle, same tool, a second time? The top of the bore in question would remain the same but the bottom would more likely "fall into place" as it's experiencing less and less deflection from the rough cut. Is it worth it? I don't know, I do know this "free cut" will bring it closer to the goal without much stress on you and the cutter. Are we now in tolerance? I realize this is dry, difficult reading but works. cmelo's example helically interpolates the motion desired.

Diction here is poor. I can see it in my head yet can not express it.

Luck.