[dalianharley]

Hi all,

Totally CNC newbie here, so please pardon my noob questions.

This is my first real job for the tormach 1100 i just bought. I'm building a tube bender and need to remake a tab. I did it first using a manual mill w/ 1-3/8" drill bit but now since I got the CNC i'd like to give it a try. Here is my job plan, please advise.

1. Fixture - machine vise holding with parallels.
2. Locating - using probe to locate the surface and edges.
3. coding - write a short gcode program by first using a center bit, then a pilot hole.
4.
here is my question

can I simply mill the hole with an end mill? if so do i still need to do the pilot hole? if the pilot hole is required, what's the recommend hole size?

or should I use a boring head instead? if so, how big that pilot hole should be? my biggest bit is 1/2" in the shop. i'd have to drive 10 miles to borrow my pal's 1-3/8" bit, which i think is too big for the tormach anyway. would boring head take a long time to do the job? the plate is 5/8" thick.

thanks!

[dalianharley]

or should I just do it on the good ol' JET mill I did them the first time.

[SCzEngrgGroup]

Drill a pilot hole, larger than the endmill you plan to use. Since it's steel, you'll probably need to go up in steps. Then interpolate to final size using a spiral toolpath, full depth, keeping a light radial engagement, so you can take advantage of radial chip thinning. You should be able to run 2400 RPM, 40IPM, full depth with 0.050" width of cut using a 1/2" HSS 4-flute endmill. You will need coolant, but it should not take long at all.

Unless you need extreme accuracy on the final size a boring head will gain you nothing other than a MUCH longer machining time.

Regards,
Ray L.

[dalianharley]

Thanks for the very detailed input. I now know how to proceed. One more question - for this case, would it be easier if I create the solidwork model first and use cam to generate the code or just write the gcode manually, or with "wizard"? I only have glanced the Gcode reference but i'm comfortable doing programming work.

Drill a pilot hole, larger than the endmill you plan to use. Since it's steel, you'll probably need to go up in steps. Then interpolate to final size using a spiral toolpath, full depth, keeping a light radial engagement, so you can take advantage of radial chip thinning. You should be able to run 2400 RPM, 40IPM, full depth with 0.050" width of cut using a 1/2" HSS 4-flute endmill. You will need coolant, but it should not take long at all.

Unless you need extreme accuracy on the final size a boring head will gain you nothing other than a MUCH longer machining time.

Regards,
Ray L.

[SCzEngrgGroup]

I can't answer that question. Which is easier depends a lot on the specific CAM, your familiarity with it, and your skill with G-code.

Regards,
Ray L.

[LSM]

drill a pilot hole something like a 13/32 a little bigger then 3/8.
get a 3/8 corncob rougher plunge in the pilot hole and work out in a spiral probably have to do it in 2 steps.
then clean it up with a finishing regular end mill, or boring head.
cad cam use well it's a good chance to get familiar with your software.
3/8 is easy to drill in steel 1/2 can be done, 1 3/8 forget it.
1/2 in corncob would work also,
with hss you will need coolant coated carbide you could cut dry with air blast to clear chips
or you can drill you hole close to the edge and slot cut leaving a solid circle in the center.
3/8 or 5/16 tool diameter for the slotting method

you could just ramp in with a center cutting end mill but that takes longer
and will decrease tool life

several way to do it just depends on personal preference and what tools you have on hand

[109jb]

Since you are wanting to try out your new mill, I'd mill it using a helical tool path and a 3/8" roughing end mill followed by a finish mill to clean up the edges. Just to play around on my old round column mill, I did it in the video link below. The mill in the video is isn't anywhere near as capable as a 1100 and the cut was done with a 2 flute HSS, no flood, etc. Because of that, the feed is much slower than you should be able to get on the 1100. I think my downfeed was 0.050" per lap. It would be faster to pre-drill, but what is the fun in that.

https://www.youtube.com/watch?v=2Y5zr4cEcxs

[Hirudin]

I think the path you take to do this job will depend one what your ultimate goal is. If you're looking to learn about CNC machining and your new mill: go ahead and cut the hole using an end-mill. If you just want a 1-3/8" hole in your piece of steel: I'd suggest using the Jet.

As a newb myself, I haven't done much steel at all, so I can only give general advice about milling... Pre-drilling a hole before you start with the end mill will do a few things for you: it'll remove a decent amount of material quickly, it'll create a hole that chips can fall through, and it'll allow the end mill to cut with only a portion of its diameter instead of having to do a full-width, "slot", cut. Slotting is difficult.

If you're interested, I'd recommend checking out this series of videos by Marc L'Ecuyer (YouTube screenname: THATLAZYMACHINIST).
https://www.youtube.com/user/THATLAZYMACHINIST
Most, if not all, of the videos are focused on manual machining, but as he's an actual instructor he's better at teaching the fundamentals than many of the other milling machine-centric YouTube channels I've seen.

[dalianharley]

Ok I'm a little overwhelmed but excited at the same time. Does end mill cut more efficiently with side flutes or from the end/tip? I see some recommended cutting at full length and some choose helical tool path.

Also corncob end mill vs regular end mill, when to use which?

Again thanks for all the inputs, learning something new from every reply.

[RussMachine]

A 'Corncob' Endmill is slang for a roughing endmill.
They are the endmills with serrated flutes (Look like corncobs), and are used to hog-out material quickly.
They will leave lines on your part, and you will need to follow-up with a regular 'smooth' endmill to finish the walls.
...
I would drill a 1/2" pilot hole, then use a 3/8 endmill to circle mill the 1-3/8 hole.
You can easily do it with one endmill (2 flute, or 4 flute), and you don't really need a rougher (corncob), if you're only going 5/8 deep.
Try using the 'circlular pocketing' Wizard in the MACH control.
It will make things real easy for ya.

[mountaindew]

Hirudin, :Marc L'Ecuyer choice of music is different, hehe I do enjoy watching his videos "some of the best shop instruction I have ever found"

As for using a nice new precision cnc mill to ram out parts in steel with little experience is not something I would do.
This is like taking a brand new jeep rubicon on the rubicon trail. It can be done, even with an inexperienced driver but damage to the jeep is almost certain.
No reason to damage the jeep, take your time and drive a few less difficult roads to get an idea of the machine and how it works.
Then you can move on and know your not doing un-necessary damage or wear to your tool.
my opinion!

Otherwise a good hss end mill with some sort of ramped plunge approach into a predrilled hole in center would be my choice
mach has some conversation mill wizards to mill a circle into your material and you can avoid code if you want. "I read g-code, I write 0.00 g-code"
You need to choose correct depth of cut, feeds, speeds and all that neat stuff and of course tool height . ...
All fun stuff to learn
md


And while I typed russ also typed just about same answer above:

[adamvs]

I can't answer that question. Which is easier depends a lot on the specific CAM, your familiarity with it, and your skill with G-code.

Regards,
Ray L.

I would use CAM, even tho this is a fairly simple op. If your CAM package has a simulation feature, even better. Writing the gcode to do a spiral cut isn't that hard, but with a CAM simulation you're pretty much assured no mistakes .. and in steel mistakes that can get ugly. The CAD for this should take about 5 minutes; the CAM you may have to begin entering a tool library, but it's a worthwhile exercise.