[howecnc]

I think I want to buy some of the modular tooling but I haven't been able to find any cutting data on the system. Any one know where to look?

Basically I am cutting 3.5" deep in 1018 steel. I was thinking of getting the 16mm head with the long Mount. I am 2 days into this with the 1/2" carbide that I have and I am not half done the job yet and I am going to need new tools soon.

Any information will greatly be appreciated.

thanks,

Chris

[Wog]

Application overview

is a good place to start. (Not Tormach, but good information)

[jakemestre]

Good Morning Howecnc,
The modular tools are a really nice concept. They let you switch heads to meet a required depth. The cutting data comes directly from the insert not the cutter body. All you have to do is find out from the insert mfr. what the recommended surface footage, chip-load, and depth of cut are. This info is typically on the box of inserts and will probably be the higher end of recommended speeds.
Another useful tool is Bob Warfields gwizard. If you're not already familiar with it the software will take more variables into account such as horse power capabilities, deflection, etc.
If you haven't already ordered your tooling you might want to get a short, medium, and long holder and swap the head. I would recommend using a short modular tool for the beginning of the operation and switching to the long tool when you really need the depth. Z height repeatability should be pretty good. Hope this helps.
Jake

[howecnc]

Thanks guys,
I was planning on buying all three mounts and a pack of 10 inserts of both grades. Seems like a smart way to go versus buying solid endmills.

[Steve Seebold]

I think I want to buy some of the modular tooling but I haven't been able to find any cutting data on the system. Any one know where to look?

Basically I am cutting 3.5" deep in 1018 steel. I was thinking of getting the 16mm head with the long Mount. I am 2 days into this with the 1/2" carbide that I have and I am not half done the job yet and I am going to need new tools soon.

Any information will greatly be appreciated.

thanks,

Chris

What are the dimensions of this 3.5 inch deep pocket? Why don't you make a drilling progral to get rid of most of the material?

There isn't a cutter out there that will remove material faster than a drill.

I do it on a lot of parts. It's called "plunge ruffing".

If you post the size of your pocket, I'll do a program to show you how it's done. It's easy. You just use your G83 drill routine.

[howecnc]

It is a "c" shaped part and with the 2 halves put together form an eccentric. I thought of plunge roughing but it would need to be done with an endmill. I need this tooling to finish the part either way. Thanks for you input.

[TurboStep]

Check out the speeds and feeds before you buy. The insert tooling can rip on a short adapter but the longer adapters will add flex. I have no idea what material they are but I'm sure they're not carbide! I have to leave home right now so I don't have time to plug the values into G-Wizard but I'd recommend that you consider the massive increase in tool length compared to the short adapter.
Step

[Runner4404spd]

with cabide tooling 1018 should cut like butter. make sure your speeds and feeds are right and make sure your not recutting chips. i am assuming that your cutting this pocket at various levels? eventually it will be difficult to clear chips. having inserted tooling won't help you get the job done, sometimes it even wears faster. you should be able to rough in .5" increments until you hit your bottom and then i would leave .01 on the bottom for cleanup.

depending on what cam software your using, and if you have access to torochoidal tool paths, that would be the deciding factor whether you predrill a bunch of holes or just go after it with a high speed tool path. with high speed tool paths the cutter won't like the constant stopping and starting and varied woc if you predrill the holes.

[Steve Seebold]

Roadrunner4404spd,

These machines only have 1 1/2 HP so a .500 DOC os out of the question.

It is possible though to drill most of the material out and then use the modular tooling to plunge ruff the rest of the material out, and like you said, leave .010 to .025 on the bottom for clean up.

I run segeral jobs for which I will plunge ruff. I will even plunge ruff the outside of some parts, depending on how much material I have to remove.

When you plunge ruff 1018 steel, I would start plunging in the center of the cavity and work outward. Then you won't have a flimsy towering area left in the center that will probably cmash your modular insert.

[Runner4404spd]

Steve,

1.5 hp is plenty, you use a .5 dia 4 flute carbide end mill and go with a .5 doc and a .05 woc and use only 0.4 hp running at 2700 rpm and at 28 ipm. at least thats what my calculator tells me. again, this is using high speed tool paths. if you don't have this option then your stuck. machine ridgidity may be a problem but i don't think it will.

[Steve Seebold]

Steve,

1.5 hp is plenty, you use a .5 dia 4 flute carbide end mill and go with a .5 doc and a .05 woc and use only 0.4 hp running at 2700 rpm and at 28 ipm. at least thats what my calculator tells me. again, this is using high speed tool paths. if you don't have this option then your stuck. machine ridgidity may be a problem but i don't think it will.

OK, that's what the calculator tells you. But what does the machine tell you.

[tbaker2500]

With 0.05" WOC yes, you're right a 0.5" DOC is possible, I do it occasionally. But this machine can't handle a .5" DOC slot, which is what I thought you meant.

[howecnc]

Well, I did buy the 16mm set. The short mount performed well. I tried it 2 ways. 5% woc .335 deep an though it was noisy the insert still looked good at the end. 2500 rpms and 20 ipm.

then I tried .0625 doc and 50% woc at the same feeds and speed. It was way faster but the tip of the inserts take a beating. Both cases beat the 1/2" endmill.

I am about to try the medium mount in a few minutes.
I can't wait to try this tool in aluminum.

I would love to see a video of the machine plunge roughing steel.

[TurboStep]

I am about to try the medium mount in a few minutes.

The suspense is killing me what happened?
Step

[howecnc]

So I have used the medium mount to finish rough from 1" down to 2 1/2" down. I tried using the side of the insert first with a small step over but didn't care for the noise.

So using .03 DOC and 97% WOC at 1250 rpm's at 12 IPM the cutter performed very well and was fairly quiet. This, compared to how I was using a 1/2" endmill sticking out 2.6", was substantially quicker by an hour and a half.

I do wish I bought the next size up for this job which would have added more rigidity and another insert but I have no complaints so far. I went with the smaller size because I don't usually do work this large and so I will still be ably to use the tool in the future.

The long mount I will only be using for finishing the ID of the two halves when they are clamped together and the job is on hold for the moment for other pressing jobs.