.5 chamfer, .75 tool

[Mic6]

Well I've looked thru all the chamfer search results on here, but haven't quite found what I'm looking for, so here goes.

My part is 7075, 1.5 square, 24" long. It's held squarely in two vises fully encapsulated in jaws. (rear jaw is one piece, floater is split in the middle)

 

The v-groove is dimensioned as .50 deep from the top, and runs the entire length of the part. I have a .75 2fl carbide chamfer mill. It's defined with a .002 dia. tip. There is a .250 wide land on each side of the groove. I drew these 2 lines defining the width of the groove. (1.00) I single chained each line and chose 2d contour, Z-.5, depth cuts .3 each, by contour, tapered walls @45deg checked. It only seems to work with cutter comp off. I hogged out the majority of the material with square endmills. It makes a clean first pass depth on each side, then drops down in the center, goes down one side, stays in the center and comes down the other side. The part should have a sharp as possible inside corner. I keep getting a step in the middle of the wall. If I use cutter comp wear, it doesnt work. Is there another way I can define the tool? I have the flip the part and do the same on the opposite side. Thanks Like crazy in advance.

(yea, I've also considered form jaws to hold them at an angle and use a square em)

 

Looks like a v-block from the end(quick paint example)

 

[ 12-02-2008, 11:05 PM: Message edited by: Mic6 ]

[RobertELee]

In MCAM the only way I have found to adjust the cut on chamfer tools is to play with the major diameter in the settings. Seems kind of silly to me, I would rather be able to adjust the minor diameter and be able to see it in verify.

[gcode]

I'd old school this one..

Look at it from side view and figure out

where the C/L of the tool needs to be

to make the cuts you need.

Draw and chain the lines and do a contour toolpath

with comp off and incremental depth of cut set to "0"

You can chain all the lines in one operation and

even add loops to get both sides of the the groove

without retracting in Z.

Sometimes its easier and faster to just draw what you want the tool to do and chain it with no comp.

You can even draw lead-in/lead out moves

and add G41 and G40 by hand to get "wear comp"

at the machine.

[Hardmill]

quote:

---

I keep getting a step in the middle of the wall. If I use cutter comp wear, it doesnt work. Is there another way I can define the tool?

---

If I understand you right its probably the tool

isnt exactly 45degs.

Cut a piece of material and throw it on

a comparator.

 

 

PEACE

[Mic6]

Thats what I thought, but the line even shows up in verification, defined as 45deg.

[Guest]

you cant cut down the center without it pulling to one side

[crazy^millman]

Best bet is to get a bigger chamfer tool so you can cut it in one pass leaving .002 as the last pass to do so. Trying to match like you are doing and not having each chain broke up into places where you can adjust according to each mis match is going to be a challenge. Any side cutting like this produces forces on the side of the endmill you just have a heck of a time adjusting for. I can take a 3/4 carbide endmill and cut the side of am aluminum block and get taper. May only be couple tenths but it is taper. Now you are trying to match angles to other angles and get it perfect. I would rather clean up after cows.

[CNC PRO]

I know I am a little late on this, but I just tried what you were describing with comp/wear, I didn't get any lines between the steps in verify (didn't try on a pysical part)...had to do a little work around but I didn't have to draw any extra lines...if this is any use to you anymore HTH.

[Mic6]

Thanks for all the responses, but I just bit the bullet and made V-groove jaws to hold the part at 45 deg, and came straight in with and endmill. It's runnign really good right now.

[crazy^millman]

thanks for that breaking news.

[Bill Craven]

I placed a tutorial on the FTP site under the training files directory called: Chamfer multipass toolpath example.zip.

 

I made this tutorial for a customer who needed to cut a weld prep with a tool that was smaller than the chamfer. It was only for a single side chamfer but it should work for what you were trying to accomplish. Take a look and save it to your arsenal if you like it.

 

A sample X2 file is included.

 

PS: I really like your final solution. Being really, really old school, I appreciate using the efficient part of the cutter.

[Rick Henrickson The Boeing Co.]

I use the chamfer function all the time with comp and it always works well even if I have to multi step. the line you drive is the edge prior to chamfer I usualy use .05 tip offset unless I have a depth constraint then fill in your width you want. The tool has to be desribe right we generally have a chamfer tool with a speced flat size so we can be sure it is right since we swap tools in and out of the cell.

[Mic6]

quote:

---

thanks for that breaking news.

---

Very Funny I dont remember if I was attempting to bump or not.