Can OneCNC cut holes with an endmill?

[Malish]

I am looking for ways to justify the purchase of OneCNC for our operation (we cuerntly use BobCad) and I just came across a program that I would think that oneCNC could do much better then how I do it now.

We do alot of programing for our 2 Techno routers. They use standard G-Code but are limited to the more standard commands (mostly G00, G01, G02/03, basic G81, ect.). Also the machines only have the spindle and no tool changer, so you are pretty much stuck with 1 tool for everything you want to cut, and the tool has to have a sandard shank size (1/4", 3/8" or 1/2"). So tool selection is very limited as well.

So the program I am working on setting up is this. I have to do a series of coutner bored holes (0.281 dia hole X 1" deep and 0.75 dia c-bore x 0.06" deep). The c-bore hole is repeated 9 times on a 14.75" bolt circle with the first hole starting 20 degrees off the horizontal axis (so my first hole location is X6.930 Y2.522). So since I have to use a 1/4" tool to do all the cutting I move to the hole center, plunge down 1.5 " (the Z zero is 0.5" above my part top surface), then I move over 0.016" and do a 360 degree circle cut. This make the 0.281 hole. I then move up to Z0.560, then out by 0.234" to get me in location to do the 360 degree circle for the counter-bore.

So my question is this, can OneCNC do these moves and then pattern that 9 times around to make my holes? Right now I pretty much do it by hand in BobCad and would love to to make my life a little easier. We do this quite often on programs for our routers becasue of the tool limitations.

Thanks in advance for any info you can provide.

Tim

[HuFlungDung]

I don't know, if this is for production, you might need Featurecam to do something that complex That's a private joke, don't worry if you don't find it funny

Yes, of course you can do this in OneCNC. Set up a style for processing a given hole, in any combination of drilling, profiling, helix down, clean circle operations and save it as a pattern. Call it up again whenever you want to apply it to a new circle pattern. This way, you need not reinvent the wheel over and over.

[Malish]

Hey HuFlungDung,

I remember talking with you way back when on the BobCad part of the fourm. Good to see you still around and psoting great info!

I have a few followup questions if you will.

1) How hard would it be to setup the first hole to do the plunge, move out, 360, rise up, move out, do 360 and then clear the hole? I know if I just want to drill a series of holes I just input the drill diameter & depth, and pick the hole locations, but to do something like this is it much more time consuming? How does someone go about doing this as opposed to just a drill function.

2) By using the pattern function that you suggested does the post write that as a sub-program or can it be posted as part of the code? Would it write it in incremtal mode or stay in absoulte for all the holes? Or is it controlable to pick however you want it done?

3) When you say "Set up a style for processing a given hole" what would that comprise in this situation. Would that mean doing 2 pocket functions, one for the deep thru hole and then a second for the shallow c-bore? Or is there some other way to get it to do the moves at hole depth?

4) When using the parrten functionality would it do all the operations in one hole first before moving on to the second holes and so on?

Thanks again for all the help. If I can find a way saving time on this it will be a great help in justifing the software.

[HuFlungDung]

Hey HuFlungDung,

I remember talking with you way back when on the BobCad part of the fourm. Good to see you still around and psoting great info!

I have a few followup questions if you will.

1) How hard would it be to setup the first hole to do the plunge, move out, 360, rise up, move out, do 360 and then clear the hole? I know if I just want to drill a series of holes I just input the drill diameter & depth, and pick the hole locations, but to do something like this is it much more time consuming? How does someone go about doing this as opposed to just a drill function.

What you are proposing is actually a pocketing operation, where you open, counterbore and re-counterbore the location. Drill cycles are most typically used to move the current tool from point to point, whilst executing a machine (drill) cycle at each of those points. Indeed, you can use OneCNC's feature recognition to gather the hole centers, then do all operations at one hole, but you will be limited to basically one hole per nc "operation", instead of the whole circle pattern.
So one plan of attack for this would be to create a normal hole routine, allowing the feature recognition to create the entire list of point locations. Set up all the operations required. Now, duplicate the first op as many times as you have locations to machine. Edit each subsequent op and uncheck all other hole locations but one. Do this to every duplicate, and leave one unique coordinate location in each one.

Another way would be to pocket each location. This would be done outside the feature recognition, just a 'stock toolpath'. Set up the operations just as you wish. Then duplicate this one op for as many locations as exist. In XR3, just repick the geometry for each duplicate, which then will do exactly the same machining operations at each hole.

2) By using the pattern function that you suggested does the post write that as a sub-program or can it be posted as part of the code? Would it write it in incremtal mode or stay in absoulte for all the holes? Or is it controlable to pick however you want it done?

No sub-programs are supported in OneCNC, but some of us do it anyways, via our post, and special purpose built drill cycles. The output is always absolute or incremental per toolpath group, never a mix. But some machines have special purpose cycles which themselves, can use incremental data, whilst the main program only positions the tool in absolute.

3) When you say "Set up a style for processing a given hole" what would that comprise in this situation. Would that mean doing 2 pocket functions, one for the deep thru hole and then a second for the shallow c-bore? Or is there some other way to get it to do the moves at hole depth?

I'd probably open the hole first, then do the top counterbore, then the deeper one, since this puts the least stress on the tool and allows for the most chip removal. I would use the hole wizard if the distance between holes is short, and I would do each operation at each location, basically going round 3 times to complete the job. But as I pointed out above, it is possible to force all 3 ops at each location, just takes a few more clicks to do what you want, is all.

4) When using the pattern functionality would it do all the operations in one hole first before moving on to the second holes and so on?

The pattern template can be invoked on as many or as few locations as you like. The pattern does not store anything about hole quantities or location.