[airbrush]

Hi,

I will need to remake my z - plate for my machine so i have a bit more length to it. Fairly simple part out of 1/2 inch alum, basically just some through holes, pockets and a couple through holes that will require tapping.

My question is about the through holes i need for tapping. I'll be using a 13/64 end mill for it and the hole needs to be that dimension as well(13/64 for tapping M6 bolts). Is it better to use a pocketing routine to do those holes or is a drill routine sufficient.

I haven't got into the software yet, just installed. Just trying to get advice and feedback if one way is better than another etc...

thx

[The Engine Guy]

Use the drill strategy, you can`t use an end mill in a pocketing routine that is the same size as the hole, it has to have a lead-in so you would end up with the endmill starting outside the hole you wanted, very messy

Regards
Rob
:rainfro: :rainfro: :rainfro:

[Ben S]

Just make sure it's center cutting.

[airbrush]

sorry newbie here....what do you mean that? make sure what is center cutting...the endmill? how do i tell? Its just a flat end mill...i'm not concerned about speed of cutting, so i will do small passes.

Just make sure it's center cutting.

[The Engine Guy]

sorry newbie here....what do you mean that? make sure what is center cutting...the endmill? how do i tell? Its just a flat end mill...i'm not concerned about speed of cutting, so i will do small passes.

Look at the bottom of the cutter. if it is a 2 flute then 1 of the flute cutting edges will go to the middle of the cutter, 3 flute and again usually 1 cutting edge will go to the centre, 4 flute usually 2 cutting edges go the middle.

Having said that don`t use end mills for drilling, very bad practice, the centre cutting is really for when you are ramping or helixing into material

Regards
Rob
:rainfro: :rainfro: :rainfro:

[airbrush]

yah...i realize its bad practice to drill with an end mill...but since its only two holes i need done with it, i figured if i do really shallow step downs...0.001 or 0.002 it would be fine....not concerned about speed...just need it to be more accurate than me drilling on my crappy drill press ....(which i did last time fairly successfully...just lots of runout on cheapo drill press.)
will have to check if they are centre cutting...not sure that they are??

[MikeC8]

Use a 1/8" endmill if you want to circle interpolate the hole. I would use a 2d profile with contour ramping checked, at a 3° angle. I would not use a endmill that is the final size of the hole.

[airbrush]

if i do it with the 13/64 i can do the whole thing in one shot without have to do a tool change...just trying to keep it as simple as possible until I start understanding the whole process some more. Once this plate is machined then I will be able to do tool changes easily using the 2010 screenset for mach.
I do have some 1/8" end mills on their way, but could be a few weeks before i receive them.

[Malish]

Using an end mill to cut a small size hole is not a good thing to do. Go to the local hardware store and buy a 13/64 drill and you will have much better luck. End mills are designed to remove material with the sides of the tool, not the bottom, that is why you ramp in or drill a hole to start the end mill in. A center cutting end mill will cut on the bottom, but it's still limited. Drills are way cheaper and less likely to break making a hole.

[airbrush]

point taken

[Strip]

Not to thread hijack but more to get further elaboration, So I am machining a small part in 1/2 thick 7075 T-6. the part calls for 1 hole to be drilled and later threaded 1/2-28. I am already using a 1/8 2-flute EM. Can I go ahead and cut the hole for the 1/2-28 with the endmill or would you switch to a spot drill (I use a 3/8 90 degree milldrill) then go to the correct size drill? I guess what I am asking is will it cut precise enough to not have to do the 2 extra tool changes for 1 hole?

[jrmach]

A 3/8 inch 90 degree mill drill is not a spot drill.They may call it a spot drill,BUT I would not use it as one.The angle of a spot drill should be at the very least as wide of angle as the drill bit.If it is not,the outer lips of your drill bit get a rough going when starting the hole.Good chance of chipping the edges.
A common angle for drills is 118 degrees.A 120 degree Spot would be appropriate.
Another common angle is 136 degrees.A 140 degree would be appropriate.
If you are worried about tool changes use a screw machine split point drill.No spot drill necessary.

I would not use an 1/8 EM to do the hole.If you don't have a tool changer,you are going to need to learn to change tools quick.Use the right tool in this case a drill

[Strip]

A 3/8 inch 90 degree mill drill is not a spot drill.They may call it a spot drill,BUT I would not use it as one.The angle of a spot drill should be at the very least as wide of angle as the drill bit.If it is not,the outer lips of your drill bit get a rough going when starting the hole.Good chance of chipping the edges.
A common angle for drills is 118 degrees.A 120 degree Spot would be appropriate.
Another common angle is 136 degrees.A 140 degree would be appropriate.
If you are worried about tool changes use a screw machine split point drill.No spot drill necessary.

I would not use an 1/8 EM to do the hole.If you don't have a tool changer,you are going to need to learn to change tools quick.Use the right tool in this case a drill

I do have an ATC, I was just curios whether or not milling a hole to be fine tapped was a practice many people do. Interesting about not spotting with a mill driil. I actually purchased the mill drill for that and to chamfer with. learn something new everyday. I did have a spot drill at one time, but I crashed it. It's been a learning experience for me, but mostly I am getting the hang of it. I guess getting the proper angle spot drill will take care of that high pitch squeal I hear everytime my drill starts. LOL

[Malish]

The only time we end mills to make a hole is when the hole is a diameter we can't get using a drill and/or it's a very large size hole, usually has to be larger then 1" diameter. The reasons for this are simple in that drill bits are way cheaper than end mills and you can make a hole faster most of the time with a drill bit, especially at smaller sizes. Drilling will also give you a exact size hole without havering to make any adjustments.

[A_Camera]

It is pointless to use end mills to drill, unless the whole is large. It simply takes too long time even in soft material, like plastic, so using a proper drill is a much better idea.

[Malish]

It is pointless to use end mills to drill, unless the whole is large. It simply takes too long time even in soft material, like plastic, so using a proper drill is a much better idea.

I do drill holes in plastic part on our routers using single flute Onsrud O-Flute cutters. The high helix make them perform like a drill in plastic and then you can mill with them as well. It's one exception that I do all the time. If you do lots of plastic parts you should check their bits out.

[A_Camera]

I do drill holes in plastic part on our routers using single flute Onsrud O-Flute cutters. The high helix make them perform like a drill in plastic and then you can mill with them as well. It's one exception that I do all the time. If you do lots of plastic parts you should check their bits out.

Interesting. I am currently making some plastic (delrin) parts which demand 7 holes with 5 different diameters, tried to win time, tested using one mill to do everything except one hole which is too small, but found that it takes a lot longer than changing tools 6 times, 5 different drills and one end mill. Perhaps if all holes would have the same depth and diameter I could also use only one end mill, but pocket drilling takes simply too long time and is inefficient compared with real drilling. At least with my DIY CNC. I have no automatic tool changer, so I try every possibility to gain some seconds or minutes. Fewer tool changing would also mean fewer Z levelling, so even there it would nice if I could work with one end mill only, but it does not seem possible to me.

[Malish]

We do mostly nylon and polypropylene material wise, but I assume it will cut very similar to Delrin will. With the O-Flute cutters I can plunge straight into the material and not have to peck like I do with a drill because of wrapping and having the material fuse to the drill bits. Also I do a ton of counter bored holes, so I plunge in the middle to full depth, then move back up and move out and interpolate a circle to make the c-bore all in one step while in the hole location. This ends up being way faster than changing tools and coming back through and spot facing for me. I highly reccomend getting one if your into cutting plastic.

Here is a link to their catalog http://www.onsrud.com/files/pdf/OC-1...oolCatalog.pdf

[A_Camera]

We do mostly nylon and polypropylene material wise, but I assume it will cut very similar to Delrin will. With the O-Flute cutters I can plunge straight into the material and not have to peck like I do with a drill because of wrapping and having the material fuse to the drill bits. Also I do a ton of counter bored holes, so I plunge in the middle to full depth, then move back up and move out and interpolate a circle to make the c-bore all in one step while in the hole location. This ends up being way faster than changing tools and coming back through and spot facing for me. I highly reccomend getting one if your into cutting plastic.

Here is a link to their catalog http://www.onsrud.com/files/pdf/OC-1...oolCatalog.pdf

Thanks for the link. Will have a look at it, but as long as I need to drill 5 different diameters, I don't think that using a single tool is efficient.

[Malish]

Depending on what size your holes are, what your tolerance on the holes is, and how thick your part is you could actually use a single O-flute to cut them all if it's a plastic material. I have done this before with multiple size holes using the same bit and interpolating the holes. I regularly cut holes in parts anywhere from 4" to 10" diameter with an 8mm O-Flute bit all the time. This is our standard bit we use for most of these large holes.

It can take longer to program but can really save you time on running, especially when you have a lot of the same parts to do. Since our routers are 4' x 8' tables to do a tool change can take upward of 20 second to go all the way back change tools and come back to the other end of the table, so for me it's worth it sometimes. The things is when you interpolate a hole your not going to get the true diameter like you do with a drill.