Plunge milling a pocket

[GeoGirl]

Hi gang,

Ok, I have a steel block 12" x 20" x 5", and a large bottomed hole about 4.7" deep for a bearing about 9" dia (has a through hole about 7" dia).

Right now I drill through, then end mill large enough pocket for my face mill and have to do this in steps.  Thoughts on plunge milling the hole. When I say plunge, I mean milling in the Z, not ramping.   I have a 1 1/2" dia 3 insert plunge cutter that is plenty long enough.  Is this wise being an internal pocket?  I don't have air, can only blast with coolant.  Can Mastercam create a plunge pocket op for me??  Using Mastercam 2019.

Thanks

Georgette

[Leon82]

There is surface rough plunge but I haven't messed with it too much. I think you have to play with the boundaries to get to do what you want. I always draw out my arcs and then sort from center out.

 

 

[Bill Craven]

There is a way to create plunge toolpaths in Mastercam that uses the legacy Ruled wireframe toolpath.  

I wrote a tutorial with a sample program for it back for version X6.

It has a lot of possibilities and versatility.  I just opened it up in Mastercam 2022.  It still works fine.

I have attached the tutorial.

Plunge toolpaths.zip

There is also a MPmaster IHS post that I modified and documented that will output feed moves for retract.

With the ruled toolpath you can create motion that will plunge straight down and then retract a small ways away from the wall and then retract to the Z clearance plane using only 3 geometry lines.  You control the stepover by changing a parameter in the toolpath.   

You can create a angled (draft) wall with 3 lines.

You can create a ramped floor toolpath.

You can create a circle plunge toolpath that will feed out in Z.  (Most tools don't like rapiding up in Z and dragging the edge of the insert)

You can create a pocket toolpath and save the geometry and use it to create a pocket plunge toolpath.  

 

These toolpaths have an advantage over drawing individual points for each plunge becasue you control the setpover amount by changing a parameter rather than drawint a new set of points with a different spacing.

 

I learned about this from a newsletter sent out by Mastercam for Version 4 (I think)  in 1990-1991.  (not X4)

Edit:  I just realized that was 30 years ago.  

 

[Smit]

We use plunge tool paths pretty frequently. They work great in the right applications, especially for machines like Haas that aren't really rigid.

Create geometry with the path you want your tool to take, chain it into a contour tool path, then use that contour tool path (turn off posting) to create your plunge tool path with surface rough plunge. Select the NCI option from the tool path, set he step over, other parameters. It's easy enough to figure out.

I expect you already know this but you'll need to keep the chips out of the pocket somehow, regardless of what tool path you choose. We have rigged up a few high pressure air nozzles to blast the chips out of places like an enclosed pocket.