Help with corner radiuses in pockets

[jspangler]

Hi

I am having a problem when pocketing. For example, I will draw a square with 1" radius corners, and then pocket it with a 1" End mill. When i chamfer the edge with my .5 inch chamfer tool, it's digging into the corners, like it's following different geometry. Is it changing the toolpath because the tol dia. is smaller?

So far it's not a problem, becasue we're welding tubes into the pockets, and covering the gouge, but why is it doing that? How can i make it copy the toolpath for the first tool exactly.

 

Thanks

 

John

[gcode]

John,

Are you using the 2D chamfer option on the contour

option page??

 

Are you sure the radius corners of your geometry are bigger than the radius of you endmill??

 

[ 12-14-2002, 02:00 PM: Message edited by: gcode ]

[P_Scott]

John,

 

Can you post the file to the FTP so we can take a look at it? Besides that, if you want an exact duplicate of the same toolpath operation, right-click in the Ops Manager on the op that you want to copy. "Copy" is part of the right-click menu that will appear. Than you can right-click again underneath the op that you're copying, and select "Paste" from the same right-click menu. You could also right-click/drag the op below itself and release the right mouse button. This will give you a smaller menu which gives you more specific choices for copying or moving the op. Then you can change the tool and Contour Type for 2D Chamfer and make sure your Depth is set to zero or you will cut deeper than you need. HTH

[Eric S.]

It could be that you tip offset is not large enough to clear the flat on the end of you tool. Check in the chamfering menu there will be two settings. One for chamfer width and the other is for tip offset. Sounds like that may be your problem.

 

Eric

[Kerry]

what i do is set my chanfering tool dia to the smallest dia od the tool..and use my z depth to make the chamfer size.. then it should be well..assuming your tool is making the proper rad and is not bigger than the corner rad your trying to produce....you might have to account for the rad on the corner of the incert for your z depth if it is too large..but it really works great and easy to compute too..

 

hope that helps

[jspangler]

Hi

The copy operation thing is what I'm doing, but I am not using the Chamfer toolpath, i'm using a straight Contour, since I'm only cleaning up the edge, not really taking anything off ( Scott Bond showed me this). I set the Z-depth by setting the tool next to the work, and seeing what barely touches. Right now I'm using a 1/2" 4 flute endmill that's been ground to 45*, following the contour toolpath, and dropping the z to -.3. The previous ops tool was 1" Dia.

 

Thanks

 

John

Hotshot Performance, inc.

[Scott Bond]

Hi John

quote:

---

I will draw a square with 1" radius corners, and then pocket it with a 1" End mill. When i chamfer the edge with my .5 inch chamfer tool, it's digging into the corners, like it's following different geometry. Is it changing the toolpath because the tol dia. is smaller?

---

Gcode asked you this

quote:

---

Are you sure the radius corners of your geometry are bigger than the radius of you endmill??

---

It still sounds likie this is a good place to start looking.

This is what I do::::: Draw some .505 corner radii so the 1" tool will turn the corner with less chatter, and then call your .5 (x90) chamfer a .250 and make it go .125 deep. In this way your are possitivly following the same geometry.

 

(slightly differant wording of the same problem)

 

If you just draw a sharp cornered rectangle, then cut with a 1" dia. you will get a 1/2' radii. Then when the 1/2" chamfer tool cuts the same internal sharp corner it will also only have the radii of the smaller tool (.250 or less).

 

[ 12-16-2002, 10:14 PM: Message edited by: Scott Bond ]

[jspangler]

Hi

Thanks. I see what the problem is now, and will go back and double check my geometry of the parts. Like i said, it's not a huge problem, but just wondering why it was happening.

 

Thanks

 

PS When are you coming around again? I have the material prepped for the mold, but haven't wanted to cut it til you were here, just in case...

 

Thanks

 

See ya

 

John