New milling motor Proxxon FBS 240/E upgrade to Kress 1050 FME-1

[JAZZCNC]

Stick to 2 flute for alu

Not always the best for Alu. It depends on the job and type of cut. If your profiling for instance and not slot cutting then more flutes are better. They allow faster feed rates with higher MRR and give better finish.
I find 3 flutes are best at roughing.? They are Stiffer and more ridged so can cut deeper. Feed rate and MRR is higher. They give a better finish if not roughers because More flutes.
The only thing is they need more attention to chip clearing and chip clearence. So not ideal for Slotting or small pockets and tight corners where tool cuts on two edges. When used with trochoidal tool paths they rock compared to 2 flute and can be run much faster with more DOC.

[Chaz]

Not always the best for Alu. It depends on the job and type of cut. If your profiling for instance and not slot cutting then more flutes are better. They allow faster feed rates with higher MRR and give better finish.
I find 3 flutes are best at roughing.? They are Stiffer and more ridged so can cut deeper. Feed rate and MRR is higher. They give a better finish if not roughers because More flutes.
The only thing is they need more attention to chip clearing and chip clearence. So not ideal for Slotting or small pockets and tight corners where tool cuts on two edges. When used with trochoidal tool paths they rock compared to 2 flute and can be run much faster with more DOC.

Agreed but generally this is good advice. I use 3 flute 8mm corn cob to rough. The rest are 2 flute.

Certainly anything higher than 3 in alu generally is a problem for most.

[Davek0974]

Great, thanks.

Things are simpler on my manual Bridgeport - just throw in a tool, set the speed to the chart and turn the hand wheels at a rate that keeps her happy :) Got a lot to learn - my reason for building a CNC partly.

So i have a g-code file from SheetCam and it was programmed for say a 6mm roughing cut leaving an allowance for finish, do i need to make a second file for the finish cut or do you use the same cutter but just program a final cut for the finish pass??

One job i have in mind has some 3mm holes in it, i would be looking at ramping in with a 2 or 2.5mm tool for them and then do the outside profile with a larger tool maybe - I am lacking knowledge of how you change tool and get back to exactly the right place OR do you use the tool dia offsets in Mach3

As i said, lots to learn;)

[Chaz]

Great, thanks.

Things are simpler on my manual Bridgeport - just throw in a tool, set the speed to the chart and turn the hand wheels at a rate that keeps her happy :) Got a lot to learn - my reason for building a CNC partly.

So i have a g-code file from SheetCam and it was programmed for say a 6mm roughing cut leaving an allowance for finish, do i need to make a second file for the finish cut or do you use the same cutter but just program a final cut for the finish pass??

One job i have in mind has some 3mm holes in it, i would be looking at ramping in with a 2 or 2.5mm tool for them and then do the outside profile with a larger tool maybe - I am lacking knowledge of how you change tool and get back to exactly the right place OR do you use the tool dia offsets in Mach3

As i said, lots to learn;)

Get Fusion 360, watch lots of good utoob vids on how to CAD and then CAM in it. Sorted.

[Davek0974]

Get Fusion 360, watch lots of good utoob vids on how to CAD and then CAM in it. Sorted.

I have that installed, trial period. I found it very complex TBH.

For what i need to do, SheetCam should be ok, I am very familiar with that as I use it a lot for my CNC plasma table, but that has no tool sizes - just the torch and that never changes size :)

Will be watching some videos though

[JAZZCNC]

So i have a g-code file from SheetCam and it was programmed for say a 6mm roughing cut leaving an allowance for finish, do i need to make a second file for the finish cut or do you use the same cutter but just program a final cut for the finish pass??

Just one file for both operations.
If corner radius are larger than the roughing cutter and the flutes edges are good enough for finish then use same tool. If not then just use smaller tool for the finish so it can clear the corners, always use a tool just little smaller than the corner radius. But in both cases it can all be done in one file.

One job i have in mind has some 3mm holes in it, i would be looking at ramping in with a 2 or 2.5mm tool for them and then do the outside profile with a larger tool maybe - I am lacking knowledge of how you change tool and get back to exactly the right place OR do you use the tool dia offsets in Mach3

With circler pockets or holes Spiral rather than ramp if possible.
When you change tools the G-code file just stops tells you to change the tool and waits for you. You then can jog the machine to easy position to change the tool. After changing the tool you reset the new Z height by touching off the material again and setting zero. Then just press cycle start and the cutting continues.
The Cam software will have taken care of tool offsets when created the g-code.

[Davek0974]

Great so I can pretty much ignore the tool offsets in Mach as it's all done in cam - program roughing cut on tool 1, program tool change, program finish cut on tool 2. Mach3 runs the roughing cut, stops and requests a tool change, I change tool and re-zero Z, press go and drink coffee ?

Now it makes sense, gets confusing when you have tool charts etc in Mach, I presume they are meant for g-code where the tool offset is not pre-programmed in cam?

Yes i meant spiral cut not ramp.

Thanks BTW

[JAZZCNC]

I presume they are meant for g-code where the tool offset is not pre-programmed in cam?

No tool offsets are for machines that have spindles with tool holders that can be changed. In this case you measure the tool length offset which is the distance from the tool tip to the surface on the holder that contacts the spindle nose. You also have the option to enter diameter for when doing tool compensation. Say for wear or under size tools.

On manual tool change spindle without repeatable holders, like ER collet system on most routers then it's not used and just leave empty. It's actually important that you don't have any values in these because if the Cam calls for G43H which is tool length compensation and theres value in that tools offset it will be applied to the tool length and change the Z height.

To see this happen do a test. Set tool #1 in tool offsets to height of 10mm and save. Then zero out the Z for tool #0 which will be the default tool when first starting mach and all offsets are referenced from.

Now using MDI type g43 H1 T1 (space between them) and you'll see the Z dro change to -10. G43 applied the tool length offset and now mach thinks the tool is at different height.! . . . Very dangerous when not being used correctly.

Don't forget to go back and set tool #1 to zero.!!

[Davek0974]

Great, thanks for that, its all starting to make sense now, surprising differences between plasma cutting and milling.

Dave

[JAZZCNC]

Agreed but generally this is good advice. I use 3 flute 8mm corn cob to rough. The rest are 2 flute.

Certainly anything higher than 3 in alu generally is a problem for most.

No it's not generally good advise because depends on the type of cut and machine, along with several other factors like cooling etc.
Slot cutting is worst case for most because chip clearence is less so people use less flutes to give more clearence. But if the machine is strong enough and cutting parameters are correct then 3 flute will work just fine and give higher MRR. It's generaly only good advise to those that don't know there machines capabiltys.!
Like wise for finishing or cutting with plenty of chip clearence like profiling then multi flute cutters work great provided the machine can handle the higher feed rates. People go wrong by using multiflute cutters is wrong situations or more often much too low feedrate. If run correctly in right places multiflute cutters give a much better finish.