Plunge cut crash

[toy4x4]

Hey guys and gals, I am having a problem with a part that I am cutting. It is a square block that I am cutting a 3D profile down one side. The problem I am having is that after a few rough cuts my cutter wants to come in over the part and plunge cut in Z directly on the part. I am using a 2.5" shellmill to do the roughing, so this poses a problem when it tries to plunge using half of the cutter. I am cutting the profile using a pocket toolpath with a containment boundry and a starting point outside my containment boundry. My use entry point is checked, I am cutting from the outside in, tool containment is set to center, and my plunge is set to outside boundry. What am I over looking that could be causing it to plunge into the part.

 

It destroyed one of my shellmills yesterday.

 

I tried to get the file on the FTP but couldn't get it to go. I will try again and let you know if I get it on there.

 

Any help would be greatly appreciated.

[Tony35]

try outside tool contaiment see if that helps in backplot

[toy4x4]

Tony, that made a difference in my backplot. It looks a lot cleaner. I will find out how that does on the next part tommorrow. Thanks for the tip.

[Tony35]

your welcome good luck

[Colin Gilchrist]

Plunge milling is very hit and miss in Mastercam. Mastercam does not understand that you have a 'non-cutting' portion of your cutter that can not touch the material.

 

I've had the best luck making multiple 2D contour and pocket toolpaths above the part, then using the plunge toolpath with the 'NCI' option (which uses a 2D toolpath for the path that your plunge mill will follow).

 

I would be very careful if you are trying to do this in a single toolpath. I've had the best results by breaking the motion up into several logical steps. Also, look at your cut depths and maximum step down. Adjust these numbers so that your tool will plunge down in a single move, without pecking...

 

One thing I've found that really helps is to disable "rapid retract" and use a retract feed value that is no more than 50-75 inches a minute. If you try to retract at rapid, it can often catch an insert and rip it out of your tool...

[X-L Engineering Corp]

Just chiming in to learn?

What’s the common practice for this method of Machining?

I’ve done this buy hand before but not fully understanding percentage of cut and Speeds & Feeds.

In Mastercam what I do is create a series of Points that I set for my step over with and then use my general speeds and feeds but someone had explained to me that the Speeds & Feeds could be much faster with this method of cutting?

Is there a better way of doing this?

 

Ted

[Colin Gilchrist]

For proper speeds and feeds I would talk to your tooling supplier. Make sure your radial depth of cut (radial engagement) isn't more than 75 % of the insert width. We were plunge roughing some nasty 15-5 forged blocks with a 2" ingersol plunge rougher. I think we were running 25 ipm for the plunge feed and 75 ipm for the retract.

 

In addition to radial step over (let's assume Y+ direction in this example) there is stepover in the X+/- direction as well. Think of this as the "plunge path direction". The step over in the plunge path direction should be about 75% of the cutter diameter (we used 1.5"), but after the cutter completes one "row", the toolpath advances in Y+ by your radial stepover amount (.25) and the toolpath then continues to step over 1.5" in X- per plunge move. It cuts in X until it reaches the end of the part, then step again in Y+ (.25), then continues to move over in the X+ direction...

 

This process repeats until you've roughed the entire part. This is the reason I usually use the NCI method for the "path" my cutter will take. I can create a Zig-zag pocket toolpath for example, with a .25 stepover. I'll use that path to give Mastercam the "radial" step amount, and in the 'Rough path parameters' tab, under "Maximum stepover" I'll enter 1.5.

 

This allows you to use a different stepover amount in your "path" direction with a smaller "radial" step amount (controlled by the spacing distance in the pocket toolpath).

 

One other trick I constantly use with Plunge roughing is to create "dummy" or "run-out" surfaces. The Plunge toolpath will not "cut" where there is no surface geometry. In order to get a good "Lead In/Out" with your toolpath, you need to create some flat surfaces that extend out beyond the boundary of your part.

 

The plunge toolpath is setup to drive the CENTER of the tool. It doesn't understand that only the inserts on the periphery of the tool are capable of cutting.

 

What I usually do is "create | rectange" and turn on the "surface" button. This lets you create rectangular surfaces that you can use in two ways: runout surfaces to extend the toolpath motion outside your part, and "check" surfaces where there is some type of shallow cavity or complex surface geometry you want to cover. By covering the surfaces/cavities you can prevent your tool from plunging into an area with the full tool diameter (ramming the tool into a closed pocket, destroying the tool and part).

 

Plunging is a great technique, but the controls in Mastercam for plunge roughing are fairly weak. I say this as an avid fan of Mastercam, but this is a glaringly weak area for the software...

[Colin Gilchrist]

One tool I'm a huge fan of is from Sandvik. They have a combination plunge rougher/high feed mill. For Cavities, you can do a helix bore toolpath using the very bottom of the insert geometry (high feed cutting) where the helix pitch is very small, (.01-.04 depending on insert geometry), but the feed rate is like .04-.08 per revolution. This makes a nice efficent entry hole. Then you can use a parallel spiral toolpath, cutting from the center out and drive your plunge path this way. Just be careful, I can not stress this enough...

[X-L Engineering Corp]

Colin,

 

Thanks for the input learned a lot with this lesson.

 

I don't know how many people use this method but were I use it the most is in thin walled parts to prevent movement. I use a much smaller amount than what you have explained but that’s because I didn't know what I was doing.

 

I use primarily Solid Carbide Endmills.

 

The next time I come across an application I will implement some of your wisdom and see how it goes.

 

Thanks again for the help

 

Ted

[Colin Gilchrist]

You are welcome Ted. I wish Mastercam had a better plunge roughing toolpath available so more people could experience the benefits. Hopefully this will help others as well.

 

Thanks,