Large chamfer with small tool

[Robert Ouellette]

How would you go about programing a large chamfer but you have to use a chamfermill thats smaller than finished size. I have a 1/4 inch chamfer to put on 3 edges of a part and the biggest chamfer mill i have is 5/8 dia. OSG with 1 insert. i am missing about .04 on rad. i know i could shift in and up and do it but there must be something in mc that would be easier

 

Thanks for all your help

Bob

[PE @ IHS]

Hi Bob

 

Please email me your file and I will see what I can do [email protected]

 

I am your contact person in the Ottawa area.

[Steel Surgeon]

How about a 2d swept tool path that way you could use a indexable cutter.

 

[ 12-22-2003, 05:15 PM: Message edited by: Newbie ]

[chris m]

Bob, if it is a relatively simple part it it probably easiest to create some phony offset goemetry for each step down and take the chamfer in 2 or 3 steps depending on what the mat'l is

 

 

C

[jbel]

+1 Newbie

 

We use 2d swept toolpaths all the time and use a ball mill or any cutter with a corner radius. A .004 or .005 step over usually suffices as long as the chamfer is not cosmetic, then we would knock it down to .001 - .002.

[Jeremy Grigsby Excelsior Marking]

This is from the help file. "A 2D chamfer toolpath places all chains at an absolute depth. A 3D chamfer toolpath, which is only available if you select 3D chains, uses incremental depths."

So this being the case, I wonder it you move your geometry 1/4" down in Z depth, if it would take multiple passes based on the tool. I haven't actually tried it but it could work. Tell me if it does.

[Jeff from MLC-CAD Systems]

Bob, I have run into this before and there is an

easy solution. select a taper tool rather than a chamfer tool and just do a regular contour ath the depth you want then, select depth cuts,select tapered walls and enter the angle of the chamfer.

works very good.

 

I put a sample file on the FTP under MC9 files

BIG-C SMALL-T.MC9 that shows this working

 

Hope this helps...

 

Regards

Jeff

[robk]

If it's a simple 45deg. chamfer, just adjust your stock to leave. Copy the operation after itself (or using depth cuts). If in your original operation you are going to finish depth leaving a scalloped sharp edge on top of the chamfer, in the second operation leave .04 in Z leave -.04 in XY. That will blend a 45deg. chamfer.

 

[ 12-23-2003, 09:35 AM: Message edited by: robk ]

[PE @ IHS]

Hi Bob

 

I received your file and sent you a response. In case you didn't get it, here it is.

 

I believe your problem is in the tool definition. You are using a single insert chamfering tool. You have defined the shank diameter and the angle correctly, but left the tip diameter as zero. This is a common mistake, with the tip being sharp, people presume that the tool needs to be defined as sharp.

 

The parameter should have the "land" diameter. Take the tool and manually bring the machine Z axis down to the workpiece so it just barely touches the surface. Turn the spindle on and you will see a small circle being scratched into the workpiece.

 

That circle diameter is the value that needs to be added into your tool parameter screen, otherwise your tool is not properly defined and the chamfer might not come out correctly.

[Robert Ouellette]

Thanks all for your help. I ended up doing as ROBK said. worked great. blended perfect.

 

Thanks again

Bob