Plunge roughing insight sought...

[danielm]

The topic says it all. I'm hoping to hear about cutters, technique, & toolpath used.

 

I've seen crazy removal rates using this but never really got into it myself.

 

 

Thx.

 

 

==> For Steel.

[Reko]

I have used Sandvik plunge mills, 4" diameter, .600" step over, 2/3rds of the cutter engaged. We had Sandvik tech's here for speed and feed recommendations, we were milling die steel and we ended up at 260SFM or 250 rpm's and a feedrate of 12 ipm.

 

Having said all that, I am not a big fan of plunge milling. We were told you can mill railroad cars full of chips per shift and that it was the best thing since sliced bread, but it left me unimpressed. I ran the plunge milling numbers in Mastercam against Sandviks high feed cutters, 4" diameter, .070" doc at 2/3rds step over, and the numbers were pretty comparable.

 

The insert cost was the deal breaker. The plunge mill inserts were $20 apiece and we changed them so often that we were burning up several hundred dollars per shift. The feed mill inserts lasted much longer and were much cheaper.

 

I am not saying you should never plunge mill, because I still use it when he application makes sense... one time, I used it to machine some rings that were a bit flimsy, and because the cutting forces of plunge milling are straight down, I supported the part from underneath and the plunge milling worked better than any other application would have.

 

The big chips coming off the part look mighty impressive, but run the numbers and you'll see what I mean.

 

What I am saying is, it is not a magical new way to remove stock that will outperform other methods by leaps and bounds... if anyone tells you that, they are just trying to sell you cutters and inserts.

 

JM2C

[Chris Bloedorn]

When you are plunge milling you can set a retract at an angle so that your cutter does not rub straight up the plunge you just took. This will increase the insert life tremendously. Not sure if Reko used this method but it certainly helps cutter life.

[HMI1953]

When you are plunge milling you can set a retract at an angle so that your cutter does not rub straight up the plunge you just took. This will increase the insert life tremendously. Not sure if Reko used this method but it certainly helps cutter life.

 

How do yo do this? This is what our tooling reps ask for, but when we asked about it in training we were told this was impossible to do.

[rogkick]

Click the Direction button in the parameters - you set the angle and length of retract.

[Jayson Kramer]

Click the Direction button in the parameters - you set the angle and length of retract.

Won't do it tried this as I was thinking about that.

[rogkick]

Jay, I don't want to disagree...but I did this last week, unless I misunderstand what he is looking for? (I am offsite so cant post the mcx file)

1. Plunge

2. Back off from Wall

3. Rapid Retract

4. Reposition

N11 G0 G90 G54 X-62.004 Y-75.351 S950 M3

N13 G43 H23 Z50.

N15 Z1.

N17 G1 Z-33.405 F260.

N19 Y-75.42 Z-31.406

N21 G0 Z1.

[DavidB]

http://www.sandvik.coromant.com/en-us/knowledge/milling/application_overview/holes_and_cavities/plunge_milling/pages/default.aspx

 

 

HTH

[DavidB]

When you are plunge milling you can set a retract at an angle so that your cutter does not rub straight up the plunge you just took. This will increase the insert life tremendously. Not sure if Reko used this method but it certainly helps cutter life.

 

I didn't know MC could do this, other CAM systems I use do it. Thanks for the post Chris is in X6 or X7?

As you will see from the post I puy above, pull away move from the vertical wall is the preffered method.

[Chris Bloedorn]

Here is a pic of the where the direction page is under surface parameters....

 

 

As far as I know the one limitation is that you can only retract in one direction...

[Jayson Kramer]

Here is a pic of the where the direction page is under surface parameters....

 

 

As far as I know the one limitation is that you can only retract in one direction...

I will try this again it kept doing it above after it was out of the cut. I thought I had done this years ago.

[Jayson Kramer]

Jay, I don't want to disagree...but I did this last week, unless I misunderstand what he is looking for? (I am offsite so cant post the mcx file)

1. Plunge

2. Back off from Wall

3. Rapid Retract

4. Reposition

N11 G0 G90 G54 X-62.004 Y-75.351 S950 M3

N13 G43 H23 Z50.

N15 Z1.

N17 G1 Z-33.405 F260.

N19 Y-75.42 Z-31.406

N21 G0 Z1.

Please do if you have it working then this is a perfect time to disagree.

[crazy^millman]

You can also do it with the lead in and lead out and just set your feed distance at the right height and it will plunge down to the contour then feed away. I have also drawn my paths to make sure I got what I wanted more work, but does ensure you get exactly what you want just use 3D in contour.

 

Now to answer your question plunge milling is a good method, but I also like highfeed milling. It really comes down to the shape and what you are doing. If doing soem crazy things like taking 12" Sqaure stock and turning it into 10" round since it is the only material you can get for a job. Flip a coin. I will say the new HS toolpaths offer a lot of options and comes down to what you want to try. A 40 taper Machine I would high Feed with High Feed inserts. A 50 taper again comes down to the part. Some areas have better results with Plunge and some with High feed. Removing materail that has no floor then plunge is a good choice if it has a floor the highfeed cutter is my choice. You can go to a floor and that is good. I have seen 16" deep plunge milling passes with no problem using a 4" cutter on a 50 taper machine. Again every situation requires you to use what is best for the application.

 

HTH

[mkd]

had some good results plunging an "F22 cord" titainium 2222 part a decade ago with ingersoll j205 grade inserts. they worked great only during full engagement plunges. cleaning up leftovers really killed the inserts.

in basic milling good ol' HSS will smoke these inserts. to me a good milling method would have worked better.

[Bill Craven]

I developed a plunge toolpath routine that uses the old Wireframe toolpaths. I placed a tutorial with sample programs on the FTP site under the Mastercam forum/training files directory some time ago.

 

The file name is: Plunge toolpaths.zip

 

You can get Mastercam to do all of the pull away or J retracts that Sandvik talks about.

 

I work for Sandvik and we offer classes several times a year on how to leverage Mastercam and NX to generate effective cutter paths which especially helpful for Heat Resistant Super Alloys.

[mkd]

forgive my stupidity, but;

if a plunge tool cuts on the bottom, the instant it is retracted the bottom is no longer seeing any wear, so how would an angular retract make any difference?

 

never mind; i guess if you had a square type insert the vertical edges dragging on the wall might be the edges you want to index to next. kinda sounds like a tool design issue? use triangular insert and go for a regular canned cycle?

i've never worried about retracts.........

[crazy^millman]

MKD, you are creating problems when dragging up the material. By the nature of the tool and process it pushes away from the Material as it cuts. When you drag up you make contact with the Material that is a much smaller cut than the cut you were taking. This will create wear conditions and possible shock or stress the insert if not feeding at the same feed rate out. I always rapid so this would crack any insert no matter the design quicker than is it was in no contact with Materail thus the move away. Do you rapid a finish endmill down the side of Material on the cut you just took to take the next one or do you move it out of the way? Same principle applies here. Moving away saves tool life and creates the best possible condtions for the tool to get the best wear possible on the inserts. More work programming yes, but when cutting Heat Treated or tough Material you need all the help you can get for tool life.

 

HTH

[mkd]

obviously i haven't done plunge roughing where you are partially engaged on the bottom while at the same time having the flank up against a wall.

i did full engagements (like a regular drill cycle) with rapids. works great. doing this in a rectangular pattern, it leaves the cusp in the middle of the four drilled areas. followed by a drill cycle centered on those leftover cusps.

thus no eccentric tool loading and NO SIDE RUBBING.

just saying this might help someone who didn't want to get involved in the fancy retracts....

[crazy^millman]

MKD we all do what works for us and gets the job done and if you get what you need and it does what you need then really that is all that counts. I am just putting my thoughts out there and hopefully they will benefit someone down the road.

[Michael Sullivan]

I'm late to the party but none the less, this works really well so thank you.

[pete_hull]

I also have mixed feelings on Plunge Milling - good on older 50taper machines that are too slow to take full advantage of more modern techniques, but big downsides as mentioned by previous posters. From personal experience Ingersoll products out performed others, typically ran 15-5ph 380sfm .006/tooth. 3.0Dia .300 stepover/ 2.0Dia .200 stepover. Must have an attentive operator as re-cutting chips was the biggest determinant of tool wear - potentially can get very ugly.

[civiceg]

I like plunging when it starts getting around 4xD deep with High feed mills, that are capable of plunging. I have had good performance on 40 taper machines, especially ones that lack rigidity. The load being axial and not radial really shines on smaller linear guide machines when the stick out is large.

 

I agree with 5 axis about the 3d contour, really makes a difference getting full control and being able to change the angle of step off depending on where you are on the part.