Newbie- Milling A2

[extrapulp]

I am trying to mill a dome shaped surface into the end of a round piece of A2 steel. I am able to create the program in MasterCam and perform the cut. The problem I am having is that the surface is not smooth. When looked at under some magnification it looks similar to the surface of a golf ball.

I have tried a 2 flute .125" carbon ball end mill and a 4 flute .25 carbon ball end mill. The 4 flute makes a better surface but seems to roll the metal off the edge leaving a burr on the entire circumference of the part.

This is using a paralell tool path with overstep of .0005" (trying to make the surface really smooth). I am taking .003"-.005" of material off the top of the part. The machine is a Hurco VM1.

Does anyone have any suggestions to make the finish smooth?

If needed I can upload screen shots of the part in MasterCam, or the dxf of the profile.

Thanks

Brian

[mc-motorsports]

by carbon, did you mean carbide? What feeds and speeds are you using now? How muc spindle speed do you have? Climb milling? Conventional milling?

Kinda sounds like your conventional milling, or using mixed direction with too slow of spindle speed.

Do you HAVE to make it out of A2? 52100 is my tool steel of choice. Easy to cut, nice finishes and gets hard as a rock after heat treat.

[extrapulp]

mc-motorsports,

Yes carbide.... sorry bout that!

Spindle speed is 4000 and feed is 30 IPM for the .125" mill, for the .25 end mill spindle speed is 2100 and the feed is 20 IPM.

I am making a punch to go in a press. We currently hand grind these A2 punches but have recently purchased the CNC mill. So I am trying to figure out how to mill the A2 punch. We have tried several different materials for the punches and A2 has given us the best results.

Thanks

Brian

[mc-motorsports]

Good tools are #1. If your using cheap tooling, the odds are against you. I use "USA Carbide", just because it's the best of what my local supply keeps in stock.

Are you roughing this out and leaving material? I would leave atleast .010 per side for the ballmill, but not more than .015" per side.

1/4" 4 flute ballmill, solid carbide, 3000rpm and 18ipm, a horizontal finishing operation will get you a better finish. I don't use MasterCam, but you should be able to tell the program you want .0001" scallop and it will adjust the step over for the angle or what not concidering the ballmill radius. You'll probably end up with a .005 to .010" step over, depending on the contour or angle, but your finish will be fine.

Climb mill only, don't conventional mill or use mixed direction. Climb milling will get you the finish your looking for, conventional milling will make a sorta chewey looking surface, orange peeled or golf balled like your describing unless the endmill is brand new. Mixed direction will get you something inbetween.

I made something probably very similar out of 2-1/2" round 52100 not too long ago. Took the part off the machine and polished it with a scotchbrite wheel for about 2 minutes and you could almost read a newspaper in the reflection. It was a form tool for use on a press, came out really nice. The first one, I made with a horizonal finish opp, then a parallel finish opp... The second one I did horizonal finish opp only and it came out a little better right from the machine. Minimal polishing and you couldn't see 1 single tool mark, just short of a mirror finish.

Your on the right track, just need to get the right parameters.

More speed, climb milling only, leave .010" material for the ballmill, you probably need more step over, let the program decide what the step over should be (.0005" step over is probably some of the problem), and lots of coolant to flush the chips away.

MC

[charger19690]

I would try what mc-motorsports says, rough it in and climb cut only..

To make dome or spherical end in MasterCam, I hardly never use Parallel, I would try Finish Flowline and play with the flow line features in the menu box when you select your geometry/ drive surfaces. You can change the start, cut direction and a couple other things. (Click on the Flowline Button)

Another thing is under the Finish Flowline Parameters tab, make sure you click the Total Tolerance tab, 1:1 and all the Create Arcs are checked. This will give you IJK or R in your other planes so it's not point to point. (Make sure your Control Definition Manager has create arcs in all planes on for your post)

Play around with that and you should get something pretty good.

Take a look at my current project at work at http://www.cncbasics.com/projects/index2.html

This guy I roughed in within .010 and used Finish Flowline with a .010 step over(just somewhere to start) and the finish is actually very good for what I am doing and I am ZigZagging, but this is Alum though too.

I think if you play with your settings some you will get there.

Mike in MN
http://www.cncbasics.com
http://www.cncbasicsforum.com

[extrapulp]

mc-motorsports - I am using kennametal tools. I guess this is a good quality tool but honestly I don't know. They are coated though, not sure if that is different than solid carbide. I will try your suggestions. Thanks for the help!

charger19690 - I have tried flowline but it gives me an error and will not create the tool path. I created the surface by drawing the profile in autocad and then opening the 2d profile into mastercam and then revolving it around. I will mess with it some more. I was not using any of the options in the total tolerance tab. I will check that out. Thanks for the advise.

It will be monday before I try again. I may need to order some tools. You guys think a 1/4" 4 flute will be better than 1/8" 2 flute?

Thanks again for your help!

Brian

[mc-motorsports]

Kennametal is good stuff! Expensive too! A kennametal solid carbide coated endmill will work perfect for your application, just making sure you wern't trying to use Emco tooling or something.

I use 1/4" ballmills all the time. I would think a 1/8" ballmill would be a little small unless you need the small tool to get into a radius. I would go bigger if anything, especially to get a longer tool.

[extrapulp]

So I was able to come up with some different tool paths this weekend, using the advise you guys gave. I came up with some pretty good results!

I do have a couple of questions tho.

I have attached a shot of the verify screen from MasterCam just to try and clarify the contour I'm working on.

The tool path that gave the best results was a spiral (edge to center) finish flowline, but it is leaving a line where it starts from the center to the edge. It does not show up in the model but does on the finished part. This is using the 1/8" 2 flute ball end mill. I have ordered 1/4" and 3/8" end mills that should be here tomorrow.

I didn't see an option for climb milling for a flowline contour. If it isn't a setting is there a way to run the tool path to make sure that it is climb instead of conventional? The finish with this tool path was not rough like before.

Thanks again for all the help!


Brian

[mc-motorsports]

The "line" you are most likely seeing and referring to on your part is where the tool path starts and stops, even if it engages and retracts for every level, or to change direction, your machine stalls for a split second and the endmill basically has no pressure on it and digs in those extra couple of thenths of a thou and leaves that visable line. My advice, polish it out unless it's excessive, then you'll have to change something to try to minimize it, could avoid it if you can change the start point of each level? I know I can't do that with my CAM system. Another cause may be excessive cutter flex, bigger ballmills will help with that, should be less anyway.

Can't help you with the MasterCam stuff, I'm sure Charger can though. But you should have a cutting direction option somewhere.

MC

[charger19690]

Brian,

Take a look at the following pics...

This was just a quick draw up, but in...

Pic1 - The flowline options menu. You get this right away when you select drive surfaces/faces and also you can click on geometry under the Tool Path Parameters.

Pic2 - Shows the tool path options

Pic3 - Show the Finish Flowline Parameters. You said that you picked Spiral..

Pic4 - Shows a step-up toolpath

Pic5 - Shows the Gap Settings menu when you click on the Button. Play around with the "Smooth" drop down. You can select different options there, you probably have it defaulted to "Broken" try "Smooth" or "Follow Surfaces" and always check the "Optimize cut order".

Another thing to do, is always go into the "Total Tolerance" button under "Cut Control" and turn the "Filter Ratio" On, and check all three boxes under it, "Create Arcs", this will filter your code at post and create "Arc" moves when possible rather then "Point to Point" code. This might help when machining it to, it will be more fluid movements for your machine.

Play around with that.

Thank,

Mike in MN

[extrapulp]

Mike,

Thank you for taking the time to create that detailed post!

I have been in all of the places you mentioned and I think I am getting that part figured out.

I have some net tooling that I have tried. A 1/8th inch 4 flute ball (Kennemetal), a 1/4 inch 4 flute ball (SGS), and a 3/8th inch 4 flute ball. The 3/8th doesn't give a good edge between the outer edge of the stock and the cut. The 1/8th ball seems to be giving me the sharpness of the edge that I am looking for and a pretty good finish. I will be trying the 1/4 ball later today.

Thanks again for all the help!

Brian

[charger19690]

Brian,

No problem, if I have the time, I will help anyone. The one thing about surfacing from my experience, because I have all on the job training, or better on the job figure it out, you just have to play with everything a bit and eventually you will get the right code and process down.

Once you do it for a bit, you will be able to just look at the generated toolpath in MC and figure if it's right or not.

Mike in MN