2d chamfer ?

[Fred @ Slate Industries]

Hello

I used to call out a .005 tool dia / 45deg

and a .125 shank and Go!

With MR2 I am getting a error

"Tool to small to create chamfer"

.015 Chamfer .03 extra tip depth.

 

Am I doing something wrong?

[?Mark]

".005 tool dia "

I hope you mean tool tip?

[Fred @ Slate Industries]

Right, Tip

[?Mark]

With 1/8 tool dia, .005" tip and 45 deg chamfer it should make .015 chamfer with no problem.

[wfcPain]

That brings up a good point.

How do you get a chamfer mill to cut using the diameter and not the outside diameter.

I always lie and say the outside diameter is .001 bigger than the diameter on a chamfer mill.

Otherwise the you have to cheat on the x y z stock to leave to adjust.

[?Mark]

quote:

---

How do you get a chamfer mill to cut using the diameter and not the outside diameter.

---

Not sure of what you mean here.

 

In his case, he can do .030" chamfer max.

.125(dia)/2 - .005(tip)/2 -.030(tip offset) = .030"

[wfcPain]

I want the chamfer mill to mill using the nose diameter , not the outside diameter.

Without changing the xyz stock to leave values.

Why not have a setting to switch between the two in the define tool.

That way you could just put in a -.032 for a 1/32 chamfer.

[?Mark]

You can't use chamfer toolpath that way, but what you can do is use contour toolpath and set tool dia = tip dia and adjust depths. It should verify ok, but I don't recommend going that way.

hth

[Fred @ Slate Industries]

I sent it in

Stay tuned

[wfcPain]

When setting outside dia (tool dia) and diameter (tip dia) as the same you get a error everytime you backplot.(Invalid tool definition. backplot will show a invalid tool). as you probaly know.

 

What i'm saying is I would like to use the nose dia as my tool diameter and still have it backplot with the correct looking 45 deg tool in backplot without fudging the numbers to make it work.

Lets say a .62 nose dia and a 1.4 outside diameter tool.

Programing off the .62 dia would make it easier imo.

You could just enter a depth of -.032 to put a 1/32 chamfer on a edge.

[wfcPain]

Thanks tony

[?Mark]

quote:

---

When setting outside dia (tool dia) and diameter (tip dia) as the same you get a error everytime you backplot.(Invalid tool definition. backplot will show a invalid tool). as you probaly know.

---

You're right, but thats not what I meant

You can use face mill that way, say tool is 2" dia, 45 inserts and has 2.5" outside dia. Will verify and backplot o'k.

Still need to adjust depths though...

[Fred @ Slate Industries]

It works fine..

I had my tool called out as taper mill

(which, even though the same geo.)

will not work.It has to be a Chamfer tool.

 

MC support

[3rdstring]

quote:

---

What i'm saying is I would like to use the nose dia as my tool diameter and still have it backplot with the correct looking 45 deg tool in backplot without fudging the numbers to make it work.

Lets say a .62 nose dia and a 1.4 outside diameter tool.

Programing off the .62 dia would make it easier imo.

You could just enter a depth of -.032 to put a 1/32 chamfer on a edge.

---

Isn't that what 2D chamfer does?

 

[wfcPain]

Imo it is easier/faster to use contour and have the tool def setup to use a chamfer mill.It just would be nice to see it backplot correctly.

You are correct. that is what 2d chamfer is for.

But its one more step and a couple of numbers to screw up....

[Storkman]

+1 to Tony. I always define it as a 45° taper instead of chamfer.

[?Mark]

?

[WWFCAM]

same problem here

 

what I did was to define the chamfer tool as a facemill and then use depth cuts with taper walls to allow for multiple depths, if the tool is defined accuratly and the taper ie 45 deg. is a true angle then the steps on the angled face are usually minimal

 

hth

[Matthew]

I use 2D Chamfer all the time with a tool defined as a chamfer tool. Usually 1/4" dia or 1/2" that comes to a point. I set my depth to INC 0.0", then in the 2D Chamfer boxes I set my tip offset .05" and width of chamfer .02". Obviously the wider the chamfer the larger the tip offset. These values will cause my tool to go to .070" deep and give me a .020" chamfer. I find it works flawlessly.

[ToolMan184]

+100 Matt. Thats what I do as well. Never had a problem yet.

[Rick Henrickson 65]

I Think the 2d chamfer mill works flawlessly to, lots of times I want to just use the very top edge of the tool to deburr closer to a vertical wall so if the tool dia. .25 I will say .005 chamfer with .12 offset if sharp tip always works great

[88Matt]

I also love 2D chamfer as well. it is a simple adjustment not only for chamfer size, but where along the cutting edge I am cutting. I can get maximum life out of my cutters with a simple number to work with.

[Steve Landkamer]

+100 for Chuck and Matt.

 

2D Chamfer works great you don't have to trig out the depth or any thing. One tip I give our customers is set your "Depth" to Abs and the "Depth" should be where the top edge of the chamfer lies in Z. Then set the chamfer dialog to the chamfer size and how far away you want to keep the tip of the tool away.

 

I did not get any error on how Tony described his tool or chamfer settings.

 

Steve

[Matthew]

quote:

---

set your "Depth" to Abs

---

This is fine if all the edges you want to chamfer are at constant Z depth, however if your edges are at multiple heights, or you are doing a 3D chamfer then INCremental "0.0" is the only way to go.

[Steve Landkamer]

+200 for Matt.