smooth 3d surfacing?

[Rich05]

x2

need to make smooth walls such as on a bowl. aluminum 6061 does anyone have tips. So far even with ball end endmill only getting steps, either that or a 20 hour operation.

need nice smooth flowing arcs on z to x and y.

the parts are all about 1 to 2 inches high and about 5 inches long 6061. not using VMC or flood, can not really high speed cut.

[kprice1658]

I'm going to jump here also. I've been playing with this piece for 3 days. I can't seem to find a good compromise between finish and speed. I machined a test piece to see if would look similar to the verify - it did. I've lost count of the combinations of toolpaths / stepovers / tolerances that I've tried.

Maybe someone can help us out?

Kevin

[makingchips]

Ok your step over is way off. Try a surface finish contour turn filter on in filter options select all the create arc boxes XY ZY ZX 3:1 tolarance of .001

Now select a 1/4 ball endmill to do the job in surface contour tab set max step down to .001 click the brokin option and on the left check the optimize toolpath. on the top click the one that says max step over set to .001 I'm doing this from memory so I might be a little off. make sure you select the top surface (flat one ) as your check surface.

Please post a picture of said toolpath after you verify.

Making Chips

[Chuck Reamer]

Originally Posted by Rich05 x2 need to make smooth walls such as on a bowl. aluminum 6061 does anyone have tips. So far even with ball end end mill only getting steps, either that or a 20 hour operation. need nice smooth flowing arcs on z to x and y. the parts are all about 1 to 2 inches high and about 5 inches long 6061. not using VMC or flood, can not really high speed cut.

For this you need flood and at least 300sfm for HSS, and 700-1000 for carbide.

One roughing pass, one semi finishing pass with about .05 DOC, and one finish pass with about a .005-.007 DOC. Set your finishing tolerance to .001, and scallop height to .0001 and it is still going to take a long time to do.

Depending on actual part size try to use maby a 1/2 ball for roughing then use the same smaller dia for semi finish and finish.

What kind of mill are you running with? What is your max rpm and IPM?

Originally posted by kprice1658 I'm going to jump here also. I've been playing with this piece for 3 days. I can't seem to find a good compromise between finish and speed. I machined a test piece to see if would look similar to the verify - it did. I've lost count of the combinations of tool paths / stepovers / tolerances that I've tried. Maybe someone can help us out? Kevin

Hey Kevin what are the rough sizes of that part, I cant look at the zip for I don't have MCAM on this PC. Use the same type of parameters I suggested for rich05, just adjust the SFM accordingly to the material type.

I found that finishing going across and not length wise makes a better surface finish.


Both of you may want to go to the Haas website and check out there magazine Vol 10 Issue 34, there is a great article on surfacing using Mastercam.

Here is the link
TIPS AND TRICKS
FOR 3-D PROGRAMMING

[Rich05]

Hi,

I am using Industrial Hobbies 3200 rpm, 2 hp motor. Having mist but do not have flood. Can you attach a sample mcx file?

Thanks!

R.

[makingchips]

Alse use a 4 flute carbide endmill S6500 F45. coolant or air blast is a must.

Making Chips

Scratch that did not see above 2HP 3200 rpm.
Also you do not need a roughing toolpath because the step down and step over is so small.

[cadcam]

makingchips why would you use a 4 flute he is cutting 6061 alum. use a two flute carbide or a 3 flute high spiral from Destney tools.

if you are using a 1/4 ball use Surface scallop and use a .004 to .005 step over and you should be able to use scotch brite to clean it up.

[cadcam]

Chuck reamer, I like you ling to the Haas surface info. that my buddy John Nelson wrote. he now head of aplacations when he wrote it he was one of the aps guys.

[Chuck Reamer]

Originally Posted by cadcam Chuck reamer, I like you ling to the Haas surface info. that my buddy John Nelson wrote. he now head of aplacations when he wrote it he was one of the aps guys.

I have that issue in print and it really helped me when I started doing 3-D surfaces. It would be damn nice to have a buddy like that, I could sure learn alot. Then again thats what CNC Zone is for, right.

[makingchips]

Originally Posted by cadcam makingchips why would you use a 4 flute he is cutting 6061 alum. use a two flute carbide or a 3 flute high spiral from Destney tools. if you are using a 1/4 ball use Surface scallop and use a .004 to .005 step over and you should be able to use scotch brite to clean it up.

Well for starters 4 flute leaves a better finish and is more rigid with the speeds and feeds supplyed. Try it you might be amazed. I know most Machinist would say 4 flute in alum. thats crazy it will gum up and break.
I do a lot of compression molds and when I set up I only want to set up once. We prove out our program on 6061 before we make the steel mold (cheaper mistakes ) Then if the program proves out I only have to change the speeds and feeds and add a few spring passes (more productive) So this is what I have found to be a good chipload for the 4 flute in aluminum.

Regards
Making Chips

[kprice1658]

Heres a pic after using 'Making Chips' suggestions. Still rough around the edges with toolmarks and a run-time of 2hrs 18 mins. I also used a 1/8" ball endmill instead of a 1/4" because of the part size - which is only 3-1/2" long and .375 diameter - so cavity is only .1875 deep & wide.

I am going to try to start with a rough cavity 1st, then try to follow up with the surf.finish.cont.

This mold will actually end up being a 4-cavity mold, so that would end up being over 9 hours to run it. I hope I can get it down - be hard to make any money only cranking out 1 mold per day

[makingchips]

Originally Posted by kprice1658 Heres a pic after using 'Making Chips' suggestions. Still rough around the edges with toolmarks and a run-time of 2hrs 18 mins. I also used a 1/8" ball endmill instead of a 1/4" because of the part size - which is only 3-1/2" long and .375 diameter - so cavity is only .1875 deep & wide. I am going to try to start with a rough cavity 1st, then try to follow up with the surf.finish.cont. This mold will actually end up being a 4-cavity mold, so that would end up being over 9 hours to run it. I hope I can get it down - be hard to make any money only cranking out 1 mold per day

Looks a lot better try running a sample part the ridges on the part might be your video card chances are they will not show up on the part. also 3D machining is time consuming its a lot more work than people think for the machine,
Ill get you close the rest is up to you.
Good luck

Making Chips