Creating a 45 deg chamfer larger then my tool

[within a thou]

I did a search for thios and found some work arounds that were posted about 9 years ago so I was wondering if there are any better solutions to this.

 

I am trying to create a 45 deg chamfer that is larger then my tool but havent been having much luck. In the past I would just run a 3d parrallel pass and be done with it since it usually was a one off job so a few extra minutes on a cycle wasnt reeally a issue but I have a decent amount of these and instead of contuosly using a bad work around I was wondering how we go about doing this. Without having to lie about the tool definition or create a whole bunch of geometry and cutterpaths to get the tool to step over properly.

 

Is there a easy way to accomplish this? Thanks in advance for any and all help.

[gcode]

make an undefined tool that represents your chamfer mill

draw a chain at the outside of the chamfer

use the contour toolpath/ depth cuts with angle (45°) turned on

set your depth cuts and leadin/out as required..

 

You really don't even need the undefined tool.

you can lie and use an endmill with the diameter set to the bottom flat on the chamfer mill

The gcode will be good, but verify and backplot won't be right.

[specv]

I use stock to leave, using multiple tool paths. I don't really draw any more geometry or change the tool definition. Its at a 45 so leaving .1 in the floor and -.1 on the wall will make another pass.

[Mr. Wizzard]

^^^^that's the way i've done it^^^^^^

Chain the edge and use stock to leave, depth cuts, multi passes.

Swap back and forth to get the size you need.

XY +.100, Z -.100 then,

XY -.100, Z +.100

[within a thou]

you can lie and use an endmill with the diameter set to the bottom flat on the chamfer mill The gcode will be good, but verify and backplot won't be right.

 

My chamfer mill has a radius at the bottom of the insert so wont using this approach give me the wrong size chamfer since it will be thinking the flat minor diameter is sharp and not offset for the tan of my radius. I am actually surprised this isn't a toolpath included in mcam its a bit hard to believe others don't also struggle with this. It would be one thing if I was on the machine but being in the ofice I can just imagine the mess I will be walking into tomorrow morning with improper tools on the set ups sheets and asking guys to comp and shift things to make it work.

 

I do realise this is "a chamfer" but we do a lot of oblong chamfered slots that are used like taper locks to lacate different parts of our assembly and it would be nice to not have to use up any of the aquimilative tolerances of the assembly if I don't have to.

[gcode]

Once you get an undefined tool that accurately represents your chamfer mill,

oversived chamfers are as simple as a contour toolpath.

Depth cuts , rough and finish

and multipass rough and finish are all there with no trial and error

about over/under stock to leave.

Its a little more work to get it going, but once the initial work is done, it works very well.

[within a thou]

How do youi add the minor in the Undefined tool dialougue I only see tip angle unless I am on the wrong page.

 

Right now I have my tool properly drawn as a chamfer mill. Using 2D contour with tapered wall and it snaps to my major diameter. So I tried subtracting my minor diameter from the major divided by 2 (to get the difference of my 2 radii and) set that as negative stock to leave. Which you would think would offset from the major to the minor and start the cutter on the minor. Through verify it was no go if undercut the part. so I stopped my backplot and measured the distance from the edge of my cutter to the wall of my part and used that to change my stock to leave. (XY-.2821)

Now verify comes out perfectly on my screen but I am a bit worried about whether the verify is correct or if the initial math I did which does not verify correctly is the correct value and before I break out the paper and calculator and revert back to do all the trig. I was hoping there was something I was doing wrong.

 

Thanks again for your patience and all your help.

[gcode]

draw an accurate profile of the tool ( not scaled) and save the file in your tool library folder

create an undefined tool (not a chamfer mill) and select that file.

set the diameter as the intersection of the bottom and angled side (sharp point) on the tool and leave the radius setting at zero.

 

when doing a contour, you chain the chamfer , not the original hole or pocket.

then set depth cuts and turn angled walls on.

 

 

[[email protected]]

HTH

CHAMFER MULTIPASS TOOLPATH EXAMPLE.MCXcreating a chamfer toolpath where the chamfer is larger than the edge of the cutter.pdfHere is a method of creating a chamfer toolpath where the chamfer is larger than the edge of the cutter.doc

[gcode]

nice..I never thought of using a taper mill definition.. thats much easier than building an undefined tool.

[within a thou]

Thanks again for all your help I will go draw up my tool.

[within a thou]

Gcode this may be a dumb question but what plane should I draw my tool in? Should the cutting edge be facing in Z- direction as it would in the mill?

[Newbeeee™]

Keith, Thanks for the file & docs

[gcode]

Gcode this may be a dumb question but what plane should I draw my tool in? Should the cutting edge be facing in Z- direction as it would in the mill?

 

 

Top plane.. with the c/l at X0 and the bottom of the tool at Y0

You only need to draw a half profile

 

check out Keith's files.. he's got a MUCH simpler way to do this

[within a thou]

Yes the taper mill worked like a charm thank you Gcode and especially Keith for the tip. Guess I have some "chamfer mills" I need to convert over.

 

Thanks again

[gcode]

Guess I have some "chamfer mills" I need to convert over.

 

keep one thing in mind.. a chamfer mill defined as a tapermill will not work correctly

with the chamfer option in a contour toolpath.

You need to keep 2 copies of the tool

one defined as a chamfer mill for regular chamfer work

and a 2nd defined as a taper mill for oversized chamfer situations

[westerfieldc]

Why not just call you tool a face mill then use depth cuts with a tapered wall?

[mchin-pilot]

Keith -Murray Mold, good effort!! v nice presentation. This is the way to teach.

[[email protected]]

Thanx guys, but I can't take credit for that. I d/l'ed it somewhere........I just can't remember where or I would pass the credit on th the respectful owner.

I am glad it helped other folks besides me tho.

[kushnercm294]

THE INFORMATION WAS VERY HELPFULL THANKYOU FOR TAKING THE TIME TO POST

[Guest MTB Technical Services]

make an undefined tool that represents your chamfer mill

draw a chain at the outside of the chamfer

use the contour toolpath/ depth cuts with angle (45°) turned on

set your depth cuts and leadin/out as required..

 

You really don't even need the undefined tool.

you can lie and use an endmill with the diameter set to the bottom flat on the chamfer mill

The gcode will be good, but verify and backplot won't be right.

 

If you define the chamfer mill as a custom tool with its diameter from the pilot end, it will simulate correctly with your method.

I use this method all the time.

[Bill Craven]

The chamfer multipass example was a tutorial that I wrote for a customer when I was a dealer. It has been on the FTP site for a few years. The reason that I included the Word doc version of the tutorial was so that if someone comes up with a better tip or wants to add their own notes, they would be able to do so.