Joining the CNC world

[Al_The_Man]

Just a tip, those amphenol connectors require a special crimping tool, which is very expensive... think it was over $200 when I was looking. .

They can be had on ebay for ~$12.00.
Al.

[Brian L]

Looks great! You can modify your G83 line to have it stay closer to he part. First, your first line of code would look like this:

G00 Z.1 (rapid down to .100" above Z0)
G99 G83 X0 Y0 Z-.7 R.1 Q.35 F10 (you could change your R level here to be closer if needed, especially if that pocket is say Z-.25)
X-10
X-20
Y-6
X-10
G98 X0 (the G98 will have the machine pull back up to the initial level)
G80 (cancels the canned cycle, otherwise it will try to drill a hole at your safe index position)

[tlowe]

Thanks Brian, that is helpful. Tonight, I will take a pic of my simple program and post it up. It works , but I am sure it is wrong and can be better.

[Brian L]

Be glad to help.

[tlowe]

OK, here is the code I had that worked except for the end of it not stopping correct and the depths of peck being off.


And here is the modified code with Brians help.


It is much faster. Does it in 1.45 minutes. And stops correctly.

[Brian L]

OK, there are millions of ways to program and none are really "wrong", but this is the way I would do your operation. First, I set my Z0 to be with the Z axis all the way up at home position. then I get a tool length from home position down to whatever I'm calling the Z0 on my part, in your case, the surface you are going to drill, or maybe the top of that lip that surrounds the valve cover, so you don't run into it. I always put my start/stop position in the program, so in case I have stopped the machine part way thru, the first thing it's going to do on a restart is move back to the beginning. Here is what I would use, I'll put the reasoning for the code in parentheses on each line. I hope this helps.

(File name: Valve Cover.tap)
G20 (sets units to inches)
G00 G40 G50 G70 G80 G90 (this is my safety line, cancels tool offsets, canned cycles and the likes)
G32 (this calls the spindle to tool change position, all the way up)
G00 X5 Y2 (your start/stop position, don't need a Z as you are already up at Z0)
(operation: drill bolt holes, T01 .281 Drill) (just a description of the tool and operation)
T1 M06 G43 H1 (Tool call, tool change, M06, which you wouldn't need if this is the only tool for this operation, G43 is length offset, Hi is this tools length in the offset tables)
M07 (mist coolant on)
S1500 M03 (turn on the spindle)
G00 X0 Y0 (move to first drilling position)
G99 G83 X0 Y0 Z-.65 R.1 Q.35 F5 (drill first hole and the G99 will keep the spindle down at Z.1 when retracting)
X-8.8 (next hole, don't need the Y if it doesn't change)
X-13.84
X-22.64
X-20.12 Y-4.311
X-11.32
G98 X-2.52 (last hole, use G98 and it will retract higher, to the initial Z level before activating the canned cycle)
G80 (cancels canned cycle)
M05 M09 (turns off spindle and coolant)
G32 (retracts to Z0 or tool change position, if it's different than Z0)
G00 X5 Y2 (rapids back to your start/stop position)
M30 (end of program)

[tlowe]

Nice.
Next question , need to drill 1.25" deep holes in cast aluminum for a bolt pattern. What method would you use? I noticed when doing the VC ,the bit would slightly drift. I want the holes to be straight.

[Brian L]

Hard to say what's causing the drift, but first thing I would do is center drill the holes to begin with, that will prevent the drill from walking about. So tool #1 would be a center drill, then pretty much copy the program with T02 being the drill diameter. You might want more rpm.... I drill 3/4" holes at 1500 rpm, little holes like you were drilling would be more like 3000 rpm, peck about every .25-.35 and keep the federate relatively slow, like 10ipm or so if the part is flimsy and has any chance of movement.

My parts are all solid chunks, so very solid in the vise and I can romp on them pretty hard. I'd be drilling at 3000 rpm and 15-20ipm with .201 (minor for a 1/4-20 thread) or .257" (minor for 5/16-18), two common sizes I drill a lot.

[tlowe]

Can you show me a example of a "center drill"? Do you mean like what is used on a lath to center the tailstock nose into?

[Brian L]

Yes, that's called a combination center drill. You can use that, or a 90º spotting end mill, which is what I use a lot, because then I can chamfer profiles and holes on the part with the same tool.

[tlowe]

So on a 9/32 hole a 3/16 center drill sufficient?

[Brian L]

1/4", 5/16" or 3/8" would be better, the point on them is smaller and you only drill deep enough to get the 60º portion out to about the same diameter as the drill bit, maybe slightly larger so it leaves a chamfer around the hole, at least you could with the 5/16 and 3/8. Whatever you have will work. I have an old 7/8" 2 flute end mill that was ground to a 90º point that I use for most of my spotting and chamfering. It is my "go to" tool for the mill because it can do so much with one tool.... I get tired of manual tool changes, so if it can give me two or three functions, a tool becomes my favorite real fast.

It is also real easy to calculate the diameter of spot drill you want when it's 90º, say I want .300" diameter, I go .150 deep, it's half of the diameter I want.

[tlowe]

Thanks.
I hear ya on the manual tool changes. Trying to limit how many I do.

[tlowe]

At the end of January, went to Milltronics and took their SLS Conversational control class. It was very good to help me learn to use my machine better. Took my 14 year old boy to it also.
When I got to the shop, went to apply some of the new found knowledge and found my machine had no ability to do conversational programming. Called the factory and was told how to fix it. Had to go into the setup area of the software and set the "full length DOS file names" to the opposite condition( off/on) can't remember. After that we can perform conversational programs. Now getting a better handle on the use of it.

[tlowe]

Just a update on me and my Milltronics. Use it all the time in both converstional and with programs made using Bobcad/cam.
I want to thank all of you for the help given me since I started this. Special attention to Sporty Bob, Brian, ZZZZZ and to Allen Mullis for giving me a good post processor for Milltronics for Bobcad.

[Brian L]

Glad to be of help, always fun to see folks get into CNC and find out how much fun they can have. I am amazed at how great a group we have here with helpful information. Back in the 70's and 80's when I started CNC machining, there was no resource like the internet and help available and freely given like it is now.... pretty amazing.

[tlowe]

Alright guy's, been doing quite a bit more machining with the VKM4. Getting the hang of it.
Question- Most of my machining is of Cast alum. Facing, pocketing and profiling. Like to take .25 deep cuts when doing pockets with a .5 or .75 EM. Face at .05-.1 . Speeds range from 1500 -2500 rpm and feeds of 14-30 for lateral movement and 30 facing.

What type of cutter would be best for profiling/ pockets in speed and longevity? Recommendations. Are indexable units OK or do regular EM work better?

[Brian L]

I use a 1/2" diameter YG brand "Alumagator" 3 flute high helix end mill for 90% of my profiling and pocketing. Tend to run just about everything at 3000 rpm as my machine tends to get too load and the spindle tends to worm up at 4,000 or 5,000. For facing I have two shell mills, both 2" diameter, one is an old Kennametal unit that has high rake inserts, works great on aluminum. The other is a generic unit that takes APKT inserts, I buy the aluminum specific high polished inserts and it works well too.

I can face at .140 depth of cut, full width, 3000 rpm and 40-50 IPM. The 1/2" EM I can cut at .25-.35 depth of cut (for slotting) and maybe 30ipm, profiling with 40% width of cut, I can get up to maybe 1" deep and 30ipm or more if the parts and set up are solid.