Face - Dynamic Mill Help

[Rotary Ninja]

When the tool gets to the center it leaves a nub. How do you prevent this?

[CJep]

Are you using the facing tpath or a 2D dynamic?

What is the stepover?

How is the tool defined?

 

How goes it Kevin?

[BenK]

Are you using a bull endmill?

[kccadcam]

If your facemill has any radius on the inserts it treats it like a bullmill.

Dynamic facemill will not compensate for this......will always leave a nub.

[Rstewart]

I haven't hat any problem with this, I use dynamic face all the time.  My 2" 90 deg facemill is defined as a .06" CR bull Mill.   No Nubs here....

[kccadcam]

I haven't hat any problem with this, I use dynamic face all the time.  My 2" 90 deg facemill is defined as a .06" CR bull Mill.   No Nubs here....

If your tool is defined as a facemill with corner radius, (as it should be) dynamic facemill WILL leave a nub.

Why should you have to define a facemill as a bullmill?

 

Tool and holder definitions need a TON of improvement, but we've been saying that for years to deaf ears....

Define a holder? Oh you have to do that in an operation?!?!? Are you kidding me????

 

Sorry,,, ranting.......

[Rotary Ninja]

I see I opened a can of worms

 

< me frantically places worms back in can.

 

My tool is basically defined as a 2" Square corner mill. The tool itself is a Widia 90 degree face mill with sharp corners. I am running a 40% stepover. At the very end the tool lifts .020" in Z as it travels in X and Y. If I delete this .020" lift in the code I have no more nub. I do not see an option to define the lift at the end of the toolpath.

 

Are you using the facing tpath or a 2D dynamic?

What is the stepover?

How is the tool defined?

 

How goes it Kevin?

 

Going good man. How bout you? It's great to see everyone is still here. I am still piecing my life back together but will be a lot more active here soon once I get back to programming at home.

[CJep]

Worms is slippery devils, specially when yer tryin' to get em back in da can.

[David Conigliaro CNC Software Inc.]

Can someone share the file in question. I need to see how the face mill is defined. Are the face mill inserts 45 degrees or vertical, etc...

[Leon82]

I have gotten them using a square endmill.

At the end of the path in the center z starts to feed up.

If the stepover is about 20 or 30% is won't leave one.

[David Conigliaro CNC Software Inc.]

I cannot reproduce this on my examples. My examples are not square, you haven't said anything about shape. Are you talking about a simple perfect square block? I tired stepovers from 10-90% with  no problems. In the end we can only troubleshoot with real files, real examples. Please send a file.

[Leon82]

here is a screen shot of the back plot and a quick file.

the tool has moved to z.0075 and has not passed over the little nub in the center.

this is a rectangle with a 3/4 flat mill 80% stepover I think

DYNAMIC.mcx-9

[David Conigliaro CNC Software Inc.]

Thank you

[David Conigliaro CNC Software Inc.]

You are causing this problem with your very aggressive arc filter settings. Look at how compromised your motion is, you should notice sharp corners and such. You actually have your arc filter set to deviate by as much as .0475in! Yikes! That's the problem. You're giving 95% of your total tolerance of .05in to the arc filter to work with.You allowed the toolpath to deviate by as much as .0475in from the original accurately calculated motion. I set total tolerance to .005in (still loose) and gave the arc filter 50% to work with. I still got plenty of arcs and no nub.

[David Conigliaro CNC Software Inc.]

Look at this image of the aggressive filter. Top is your file as sent to me.

[David Conigliaro CNC Software Inc.]

[David Conigliaro CNC Software Inc.]

[Leon82]

Interesting. I must have set it to try and shrink a program and hit the save button.

I rarely look at the filter settings for facing

[David Conigliaro CNC Software Inc.]

At least we know why the nub is there  

[MIL-TFP-41]

Ok, I'll bite. See attached file, nub city.

High feed cutters are way easy to duplicate this problem. No I don't want to define my 2" diameter cutter as a 1.764 diameter facemill.

dynamic face.mcam

[MIL-TFP-41]

And here is why you don't want to define the facemill as a 1.764 diameter cutter.

dynamic face and contour.mcam

[David Conigliaro CNC Software Inc.]

You did not define a highfeed cutter? You defined a Face mill cutter to look like a highfeed cutter. If you use the actual HighFeed tool type we take care to comp accurately to the bottom highfeed profile. Mastercam is comping your tool as defined like a sharp endmill, the picture shows it on the definition page. Blue flutes represents your profile shape, yellow flutes represent what Mastercam uses to comp.

 

[David Conigliaro CNC Software Inc.]

There should be nothing wrong with the facing toolpath when tools are defined correctly and arc fit tolerances are reasonable.

[MIL-TFP-41]

Ok, what if my 2" diameter facemill has a 1/4" radius? Use a bullmill?

[David Conigliaro CNC Software Inc.]