PrototypeFred

How to use 2D chamfer

15 posts in this topic

Hello

Can anyone tell me how to exactly use the 2D chamfer in Contour.

Ok lets say I have a 1" bore diameter and I want to put on it a 45 degree chamfer by .010 (chamfer amount). I will be using a .250 diameter 45 degree chamfer mill. I also want to use the cutter comp. So I will set it to "wear" and compensation direction to the left. Then I select from contour type "2D chamfer" ,when I go to the exclamation point there is a window that says "chamfering" . What am I suppose to put in the width and the tip offset?

 

I know how to put in a chamfer by just sneaking up on it with a Z minus and not using the 2D chamfer . But I really would like to know how to use this feature correctly and take out the guess work.

Thanks

Share this post


Link to post
Share on other sites

the chain should be the finished diameter of the bore.

in the chamfer field, you enter the radial size of the chamfer (.010 in your case)

the other field is the vertical offset of the tool.

what's important is that the bottom size of the tool deffinition be accurate.

On the machine you touch off the bottom of the tool to set the length offset.

If you've done all this accurately setting your diameter offset at zero will give you the chamfer size you programmed.

Share this post


Link to post
Share on other sites

Hello

Can anyone tell me how to exactly use the 2D chamfer in Contour.

Ok lets say I have a 1" bore diameter and I want to put on it a 45 degree chamfer by .010 (chamfer amount). I will be using a .250 diameter 45 degree chamfer mill. I also want to use the cutter comp. So I will set it to "wear" and compensation direction to the left. Then I select from contour type "2D chamfer" ,when I go to the exclamation point there is a window that says "chamfering" . What am I suppose to put in the width and the tip offset?

 

I know how to put in a chamfer by just sneaking up on it with a Z minus and not using the 2D chamfer . But I really would like to know how to use this feature correctly and take out the guess work.

Thanks

 

 

Once you pick a chamfer mill in your tool settings the picture (in mastercam X versions) should be pretty self explainitory. The width of the chamfer you want (.010) goes in the "width" box, the tip offset is how much the cutter hangs past the bottom of the chamfer so there is an allowance to stop the cutter cutting right on the centre.

Share this post


Link to post
Share on other sites

Hello

Can anyone tell me how to exactly use the 2D chamfer in Contour.

Ok lets say I have a 1" bore diameter and I want to put on it a 45 degree chamfer by .010 (chamfer amount). I will be using a .250 diameter 45 degree chamfer mill. I also want to use the cutter comp. So I will set it to "wear" and compensation direction to the left. Then I select from contour type "2D chamfer" ,when I go to the exclamation point there is a window that says "chamfering" . What am I suppose to put in the width and the tip offset?

 

I know how to put in a chamfer by just sneaking up on it with a Z minus and not using the 2D chamfer . But I really would like to know how to use this feature correctly and take out the guess work.

Thanks

 

 

double post :veryangry:

Share this post


Link to post
Share on other sites

Also, bear in mind that the toolpath takes into account the taper angle of the tool being using. So if the tool has a 30 side angle, and the chamfer distance is .010, it will produce a chamfer of .010 from the bore size. gcode is right though, the tool has to be defined accurately.

 

It works really well. I use it all the time :)

Share this post


Link to post
Share on other sites

Ok so the tool I will be using is very sharp and really has no tip diameter in other words it has no it has no bottom diameter. So what do I put in the "tip offset" field ?

Share this post


Link to post
Share on other sites

0 WIll be your tip diameter. You may have to have a value though so if it won't accept 0, then put .001 or smaller.

Share this post


Link to post
Share on other sites

Or just use spot drill and set the angle?

In the machine wear register, plus up the tool 5 thou, run it, measure the part, drop the wear as necessary, and run again.

Share this post


Link to post
Share on other sites

Ok so the tool I will be using is very sharp and really has no tip diameter in other words it has no it has no bottom diameter. So what do I put in the "tip offset" field ?

 

 

In your tool def you can't put 0, so just put a small value like 0.001" for the tip dia

 

you will still want to put in a tip offset value though as you don't want to try and cut the chamfer with the very tip of the tool as it is effectively turning at zero rpm.

 

if you are running a say a 1/4" dia 90 deg included angle chamfer mill and you are cutting a 0.010" chamfer you could potentialy use a tip offset of say 0.1" to get the tool to cut near the outside where your tool surface speed is at it's greatest. This tip offset box is very handy when trying to get chamfer mills into tight areas.

Share this post


Link to post
Share on other sites

In your tool def you can't put 0, so just put a small value like 0.001" for the tip dia

 

I use 0.

Not sure why you can't though.

Share this post


Link to post
Share on other sites
I use 0.

Not sure why you can't though.

back in the day (V9) the tool manager wouldn't accept a zero for chamfer tool tip diameter.

Maybe they've fixed it since then.. I've been using .001 for years and years.

Next time I make a chamfer mill, I'll try a zero

Share this post


Link to post
Share on other sites
Next time a make a chamfer mill, I'll try a zero

 

Just did.

 

Don't know when it was changed but now you can.

 

Back when, it would not, .001 was what you had to use.

Share this post


Link to post
Share on other sites

As a side note, I use the chamfer mill when defining spotting drills. Typically the chisel edge of a spotting drill exists, so the point diameter is something other than 0. By doing this, when I programme a spotting drill to go deep enough to achieve a chamfer for a tapped hole (or for any hole for that matter) in a drilling cycle, the verification will refelct the correct sized chamfer, and the correct chamfer will machined (it won't be too big).

 

This is especially true for smaller threads/holes

 

For example, a 6mm x 90 degree spotting drill typically has about a .9mm wide chisel edge. So I define a .9mm nose diameter, 6mm OD, with a 45 degree angle. It works like a charm :)

Share this post


Link to post
Share on other sites

I use 0.

Not sure why you can't though.

 

 

your right Jeff, good spotting, guess I would have just kept doing this for years after having to for the last 15 :thumbsup:

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!


Register a new account

Sign in

Already have an account? Sign in here.


Sign In Now

  • Recently Browsing   0 members

    No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us