Winmax and chamfer mills

[Captdave]

I'm trying to chamfer the top of a part with a 1/2" Chamfer mill. Currently I have the tool set up as a Chamfer tool, .5 DIA, 45*, Tip DIA 0. The part is set mill frame, .030 DOC, milling type outside and it Cuts air. Change to mill type ON and it cuts the chamfer but leaves a bur on the side since its not cutting past the edge.

What gives?

[glovebox20]

Hello again.

The Hurco Mills that I run have the Ulitmax III or 4 control and do not have a "Chamfer tool" as a tool type option. I'm assuming that your chamfer tool has a Major Dia of 1/2 inch and it chamfers down to a "Zero dia point" on the bottom. What I would do is call your Chamfer tool a "End Mill". Then use .060" for the dia. This way when you use "cutter comp" to mill the part (cut "left/right",mill frame "outside/inside", etc), the point of your tool would be offset .030 from the part profile (radius of the tool). However, you will have to add .030" to your Z depth in or part program to get your correct chamfer size. (.03 chamfer + .03 point offset= Z-.060"). This should work pretty good being the point is past the edge of the contour to eliminate that funny looking burr.


When you selected "ON" as your frame type, It put the center of the tool right on the edge of your profile giving out that funny burr on the edge of the part. I don't have your version of Winmax, but if you could e-mail me a .pdf file of your help file, I could read through it and see if there another way of doing it by using a "chamfer" tool type like the way you probably prefer. One more question, If your using the "solid graphics" function to draw the part, dose it show the chamfer being put on the part? It should if the tool geomerty info is set correctly and it is program right.

good luck

[Captdave]

Sounds good, I'm working on building a fixture for the thread mill and hex op we spoke of earlier. If you PM me with your email I'll send the PDF file to ya.

[glovebox20]

PM sent

[Captdave]

Email on the way, Thanks

[glovebox20]

Well, you got me stumped.

According to the "Getting started with Winmax Mill" pdf file, tale 4-1, when you pick "Chamfer Tool", it uses the tool tip dia. for cutter comp. If your using a tip dia. of "0", there should be no cutter comp. applied so weather your cutting "ON, Left, Right, Inside, or outside, it should be all treated the same and put the center of the tool on your profile. You can try adjusting your angle to 90* and see that makes a difference but I don't think it will because the major dia. and angle should only affect the solid graphics rendering.

At any rate, you can try calling your tip dia. .060" and add .030" to your Z depth on your chamfer tool and see if that works like my "End mill" example.

When you say it "cut's air", how much would you say it's cutting? If it's .250" I would say it using your Major dia. to calculate your comp value.

If your using Tool path graphics (wire frame), the center of the cutter is shown as a dotted line (red?) and your part surface as a solid line (cyan?). If your not using "cutter comp", there is no solid line (part surface). Obliviously, if your cutter is narrow, the dotted line should almost be on top of your part surface vs. a wide tool. This may also help you trouble shoot your tool path.

Good luck with your hex fixture.

[Captdave]

If I use .5 as the tool DIA and 0 for the point angle 90*and cutter comp left or right, it applies no comp as the tool is .250" offset from the part. I used your example and finished the parts so I'll have to look at the graphics another time. I may get a little more time on Monday to play with it before I head out on another trip.

Is there a support group at Hurco that I could contact about these issues?

Thanks again for your input.

[Captdave]

Well if appears that it doesn't like a tool tip of 0, but .0001" works great!

[glovebox20]

Originally Posted by Captdave Well if appears that it doesn't like a tool tip of 0, but .0001" works great!

Allright!! Thanks for the update. Must be one of those software bugs that the salesmen will never tell you.

Hurco's web site dose have a online support
http://www.hurco.com/USA/Support/Pag...coSupport.aspx
Never used it myself tough.

You can also contact your local Hurco Distributor.

Applied Machine Solutions, Inc.
1441 Airport Dr.
Suite 300
Ball Ground, GA 30107

Tel: (678) 880-0893