[chris123]

Yep Im new and still learning
This part is 6.5" x 1.5" x 10mm

I am using a 4mm flat end mill to do everything
I need to do profiling and facing
I'm currently running at 24ipm at 7500rpm and cutting 0.02" each time

Is there a specific tool bit I should be using for facing and profile?
Should I be using a larger or different toolbit? 6mm 8mm 10mm?

Here is the part



This is the machine, Taig bench mill

[christinandavid]

If you are happy with it leave it as is.

If its taking too long turn the feed up.

If your cutter burns out turn feed down, take deeper cuts.

If it breaks your cutter try a fatter one.

If it shakes your machine apart change your milling strategy.

Repeat sequence until you run out of components/cutters/money/time.

DP

[fly_boy_bc]

What is making you think that you need to use other tooling? Is it the "grooves" in the workpiece?

I have the exact same Taig micro mill that you have. I ordered mine from Microproto Systems. I have only had it a week and I am a complete noob.

I suspect that a flat end mill of a larger diameter will eliminate/reduce the scaloped effect. But I am a noob so wait for more experienced answers.

In any event I will be watching for your answers. They will certainly help me in the long run.

What is that piece you are making anyway?

Gary B in BC doing CNC

[chris123]

1. If you are happy with it leave it as is.
2. If its taking too long turn the feed up.
3. If your cutter burns out turn feed down, take deeper cuts.
4. If it breaks your cutter try a fatter one.
5. If it shakes your machine apart change your milling strategy.
Repeat sequence until you run out of components/cutters/money/time.
DP

1. It takes way too long I'd to machine it faster
2. I cant turn the feed up thats the machine max speed
3. Taking deeper cuts the aluminium just gums up jams the tool bit and breaks it
4. I will try a fatter cutter, 8mm
5. The machine is not shaking

[chris123]

1.What is making you think that you need to use other tooling? Is it the "grooves" in the workpiece?
2. I have the exact same Taig micro mill that you have. I ordered mine from Microproto Systems. I have only had it a week and I am a complete noob.
3. I suspect that a flat end mill of a larger diameter will eliminate/reduce the scaloped effect. But I am a noob so wait for more experienced answers.
4. In any event I will be watching for your answers. They will certainly help me in the long run.
5. What is that piece you are making anyway?

Gary B in BC doing CNC

1. No, its the time it takes and I cant seem to cut deeper as it just breaks the tools bits
2. This is only mill Ive ever seen and used in real life, I can not judge on how good or bad it is
3. I will try a larger end mill
4. Yep, most people here have larger mills and unless Im doing something wrong, doing what they say is not possible
5. Its a guide rail

[Algirdas]

use coolant. If You arrange just powerfull air blow, it helps very much.

[chris123]

to get it to what it currently can do i use wd40, air is not enough

[Algirdas]

just kerosine is enough. WD40 is intended for different use, too expensive here

[christinandavid]

Change your strategy to helically mill a 2xD clearance hole to full depth, then mill out the pocket required in a spiral/trochoidal fashion using the full length of the cutter but a small radial overlap. This strategy can be faster and is much gentler for the cutter/machine than a full diameter cut. Not as much heat will be generated, the swarf will then have somewhere to go, you will not knacker the very end of the cutter so much. A ripper form cutter will take more of a beating if the side finish is not too critical. If it is an end mill to finish the tab.

DP

[fly_boy_bc]

1. No, its the time it takes and I cant seem to cut deeper as it just breaks the tools bits
2. This is only mill Ive ever seen and used in real life, I can not judge on how good or bad it is
3. I will try a larger end mill
4. Yep, most people here have larger mills and unless Im doing something wrong, doing what they say is not possible
5. Its a guide rail

1...How long did it take to get to the point you are at in the pictures? Rememer it's cut deeper AND slower NOT just deeper.
2...All i have ever heard tells me that the Taig is a superior machine for the size. 1/8 inch cuts in steel with a 1/8 inch end mill. SOLID.
3... Yes that is the first thing I would try it should help the finish too. Is it a nice new sharp endmill?
4...Deeper AND slower, use correct coolant, are you using air or kerosine? WD40 is barely useful. Yes you can.
5...For what?

[chris123]

1...How long did it take to get to the point you are at in the pictures? Rememer it's cut deeper AND slower NOT just deeper.
2...All i have ever heard tells me that the Taig is a superior machine for the size. 1/8 inch cuts in steel with a 1/8 inch end mill. SOLID.
3... Yes that is the first thing I would try it should help the finish too. Is it a nice new sharp endmill?
4...Deeper AND slower, use correct coolant, are you using air or kerosine? WD40 is barely useful. Yes you can.
5...For what?

1. It takes about an hour from start to finish. The tool bit I'm using is brand new. When I cut deeper e.g. 0.03" the aluminium gums up to the point where it jams the machine and breaks the bit. Slower as in RPM and IPM
2. I think its more to do with the type of aluminium Im using, I've cut through 0.07" dry and with the same sized bit on different aluminium
3. It is new because I broke several bits before I worked it out
4. air does not work, wd40 does, is kerosine classed as correct coolant?

[awerby]

Is there any reason you're using this particular stuff? Most machinists prefer a heat-treated alloy, like 6061 T6. Non-heat-treated aluminum tends to be gummy, cuts poorly, and welds itself to the cutter

From the looks of the cut, it seems like your mill's out of tram. If there's "stair-stepping" side-to-side, then you need to square it up by loosening the nut on the back and using a machinist's square to establish a true 90 degree angle of the column to the bed. There are more elaborate tramming routines, but that should get you most of the way there.

You should do the majority of the stock removal with the largest cutter you can. There are 10mm ER-16 collets available. If you have details it can't reach, follow up with a finish cut using a smaller-diameter tool. Christiandavid had some good suggestions on this. Finish cuts in aluminum come out cleaner if you use "climb" cutting rather than "conventional".

Andrew Werby
www.computersculpture.com

[chris123]

Is there any reason you're using this particular stuff? Most machinists prefer a heat-treated alloy, like 6061 T6. Non-heat-treated aluminum tends to be gummy, cuts poorly, and welds itself to the cutter

That's most likely the problem I know the rod I machine is 6061T6 and I can cut much deeper and it does not go gummy
It's hard to find flat bar 6061-T6 aluminium in australia

From the looks of the cut, it seems like your mill's out of tram. If there's "stair-stepping" side-to-side, then you need to square it up by loosening the nut on the back and using a machinist's square to establish a true 90 degree angle of the column to the bed. There are more elaborate tramming routines, but that should get you most of the way there.

To the bed, oh yeah I was just using a spirit level to level the head. The bed most likely isnt level. I shall square it the the bed

You should do the majority of the stock removal with the largest cutter you can.

I have already ordered the larger tool bits

[fly_boy_bc]

1. It takes about an hour from start to finish. The tool bit I'm using is brand new. When I cut deeper e.g. 0.03" the aluminium gums up to the point where it jams the machine and breaks the bit. Slower as in RPM and IPM
2. I think its more to do with the type of aluminium Im using, I've cut through 0.07" dry and with the same sized bit on different aluminium
3. It is new because I broke several bits before I worked it out
4. air does not work, wd40 does, is kerosine classed as correct coolant?

1...that's only slightly longer than I would expect it to take. Slower in IPM.

2...Ohkhay different materials cut differently. This may be the best you can do with this particular material.

4...yes kerosine is for aluminum.

As the other (obviously more experienced than myself) poster says you most likely need to tram your mill based on the grooves in your workpiece but I suspect your biggest problem is your milling strategy. (As stated by the other, obviously more experienced poster). I don't pretend to understand EXACTLY what he is reccomending but I think we both get the gist "try to load the side of the cutter more,the end less and have lots of room for the swarf and overlap your rows like when cutting the lawn. Try NOT to drill holes with a mill (that's what drillbits are for) and use the SIDE to remove material as much as you can.

Gary B in BC doing CNC

[fly_boy_bc]

Change your strategy to helically mill a 2xD clearance hole to full depth, then mill out the pocket required in a spiral/trochoidal fashion using the full length of the cutter but a small radial overlap. This strategy can be faster and is much gentler for the cutter/machine than a full diameter cut. Not as much heat will be generated, the swarf will then have somewhere to go, you will not knacker the very end of the cutter so much. A ripper form cutter will take more of a beating if the side finish is not too critical. If it is an end mill to finish the tab.

DP

Hi I am not the original poster but could I ask you to re-state your reccomendations in slightly less technical language? As stated in my last post I get the general idea but I am not completely sure of some of the jargon.

2xD clearance hole to full depth?? Cutter diameter times two to the top of the piece or?

[christinandavid]

Hi,

Looking at the scenario, I assume that limited tooling and the desire not to keep changing tools may be a factor, so the point is to do as much with one tool as possible.

I would probably split the area to be machined into two or three areas - the big left-hand area, and an area above and below the tab (not sure if that tab extends full length of part, in which case two areas above and below tab).

If software is available to produce the code, and if the machine can do it, I would produce a large enough clearance as possible in each area to full depth as a starting point for pocketing. The largest this can be using a helical path would be twice the cutter diameter. The cutter would need to be end cutting, ie a slot drill where one flute extends beyond the centreline of the cutter, or an end mill with a similar form on the end (two flutes cleared to the centre). A helical path to produce the hole involves a circular move in x and y while feeding down in z.

Once these starting point clearance holes are established at the centre of each area, open out each area by climb milling out the original hole, opening it out to the eventual desired shape of that particular area. For the more proportional areas, a spiral path could be used - for long and thin areas, a trochoidal path, which is a similar concept to helical, but feeding across rather than down. This way the radial engagement of the cutter can be kept to a minimum, reducing flex, heat generated, recutting of swarf. Going to full depth/flute depth uses the cutter most efficiently.

Problem areas are corners, where cutter engagement 'spikes' and load on the cutter increases massively. A way around this, if the helical option is a possibilty with machine/control, is to helically mill the corners out along with the starting point clearance holes. With all potential 'spikes' removed it will be easy to get the cutter to its optimum in terms of feed and depth of each pass.

Of course, I'm assuming that the software/hardware being used is capable of producing these kind of paths. I am not a home machinist so I can't foresee the limitations that may be involved. I have proven out the benefits of the approach at work however. Even when times are not improved significantly, you can really see the difference on the tool.

I imagine without flood coolant swarf is a major problem to remove - is there any reason the method of manufacture could not be altered to allow swarf to escape more easily? ie machining the part at the corner of the stock or cutting out profile and removing stock before machining faces? (this would involve quite a rethink and involve putting at least one more hole in the rail to clamp through)

DP

[chris123]

As the other (obviously more experienced than myself) poster says you most likely need to tram your mill based on the grooves in your workpiece but I suspect your biggest problem is your milling strategy. (As stated by the other, obviously more experienced poster). I don't pretend to understand EXACTLY what he is reccomending but I think we both get the gist "try to load the side of the cutter more,the end less and have lots of room for the swarf and overlap your rows like when cutting the lawn.

Thats doesnt make any sense
You just said two contradictory things
The only way to make grooves like I did is to machine using the side of the bit like I do, but you mention that I shouldnt be drilling which I dont because I am making those groves

[chris123]

Hi,

Looking at the scenario, I assume that limited tooling and the desire not to keep changing tools may be a factor, so the point is to do as much with one tool as possible.

Tooling isnt limited I just dont have the tools yet, I would gladly change tools if it means the piece gets done quicker

When I get my larger end mill I shall experiment with depth and feed rates to see what is possible. What you describe will not work very well with my current set up, mainly due to the material I'm using. The software is more then capable of doing helical entries or pocketing like that and the machine can do it but this aluminium I'm using wont let it happen with much ease

[fly_boy_bc]

Thats doesnt make any sense
You just said two contradictory things
The only way to make grooves like I did is to machine using the side of the bit like I do, but you mention that I shouldnt be drilling which I dont because I am making those groves

Lighter passes (depth) heavier passes (overlap)

Load the side more and the end less. Of course you are "drilling". Every time you send your cutters face farther into the material. Reduce that but increase overlap. (This is what I gleaned from christinandavids post perhaps he could chime in again?)

[fly_boy_bc]

this aluminium I'm using wont let it happen with much ease

That is the crux of it here. Funky material.