Follow up, undercut cylinder question posted

[jgaertner]

Hello Forum,

I am working on machining an undercut groove in a cylinder on my CNC mill. I received some help earlier on the forum but wanted to explore the 3D contour Op as a possible solution. I made a 3/16 radius Convex tool (which I just learned how to do). It seems in simulation that the cutter makes a much deeper cut a little more than half way through the contour op? See attached picture of the tool path. I don't think this will work. Wonder whether I have to do it in 2 ops? Any positive suggestions will be appreciate. New file attached.   Jgaertner

[Anonymous]

So, looking at your new post and tool, I tried to get smoother transition from outer edge to start of the radius and there is just no fix for it in single tool path that I can figure out.

Marking "detect flat area" has no effect on outcome and I had really difficult time getting anything to stick, too many "internal Cam errors" and "empty tool path" flags without any clue as to why.

I then reloaded model that I modified in your previous post to make wrap tool path work and used 2D contour to rough radius and finish flat walls then finish radius using Ramp.

Tool shank was hitting top of the model OD so I made shank .7 diameter, basically you need to relieve it for clearance.

[jgaertner]

Thank you for taking another look at this challenge. I don't think I will be able to change the geometry of the tool since I would have to buy one from Travers.com https://www.travers.com/convex-radius-shank-type-high-speed-steel-cutter/p/10-271-710/  Not sure what the solution would be? Maybe some other people will have a look? Jgaertner 

[Anonymous]

Just so we are on the same page,........... if tool doesn't have required clearance, your options are to relieve shank or use different tool, not a matter of opinion.

Edit;

It looks like I uploaded wrong version of file in my previous post, I'll see if I can recover one that matches description in that post.

[jgaertner]

I would not be willing to alter a commercially manufactured CNC cutting tool. I have not found another source yet for a different convex cutting tool, with any different geometry. Could be one out there, just have not found it. 

[Anonymous]

Groove is .022 deeper then tool can reach, compare two screen shots, one has tool shank set to .75 and the other to .7.

If you leave it at .75, Fusion avoids crashing it but does not complete groove.

BTW, trying to use Shank in Ramp operation results in internal Cam error.

File attached.

 

[Anonymous]

Grinding tool shank to clear desired cut is a very common practice in machine shop, last resort,........ but done  routinely when there is no other option.

[jgaertner]

Thanks. This may not be an issue. I have no idea how you create the convex tool in your library with a narrower shank but the Travers tool has a narrow neck. see attached picture. So I need to learn how you change the shank dimensions in the Tool Creation?  I did not know how to make the tool using slotting until yesterday.

[Anonymous]

You can modify any parameter to learn what configuration works with given need, then look to buy closest possible match or modify it to suit the need, I am only talking about modifying shank, not cutting flutes.

If tool you are buying has in fact smaller diameter behind cutting flutes then the rest of the shank, that's great but you have to take it into consideration and see that it clears the model.

[jgaertner]

Yes, But I see no way to change the tool in Fusion to represent the narrower shoulder/neck so that Fusion does not program or think it will program a crash of the .75" dia. neck with the upper portion of the die? 

[Anonymous]

You can try to coordinate shaft and cutter spec's, I generally ignore settings in shaft tab and just set tool shank to what I know is critical factor in clearing the cut.

[jgaertner]

I found more details on the convex cutter. The necked down area is 5/8" and 1/2" tall. Then the shaft is .75". I just changed the tool to the .6250" diameter and I know I will have to use a .75 collect. Don't know what else to do. Funny how they show a necked down slot cutter but no way, I see, to creat one?

[Anonymous]

Tool has plenty of clearance, if you define cutter as having 5/8 shaft, it matches physical dimensions and Fusion should have no issues with completing full depth.

Simple grooving job on lathe, or using Rotary tool path on 4th axis, ...... assuming you don't have either one, just wondering.

[jgaertner]

Thanks for checking. I have a very nice Birmingham 14 x 40 lathe and could do it on the lathe, but then I would not have learned anything... my goal is to work on parts that challenge and teach me something new for future use. Will see about ordering the convex tool. Jgaertner

[Anonymous]

I was gonna say ......... "so... you like to do things the hard way" ........... but you bailed out on learning subject, (sorry, I couldn't resist).

I too am messing with things I will never actually do on machine, due to nature of my domain,... learning things is challenging and entertaining, you never know what may come your way next.

[jgaertner]

The dies area for a paying project I am working on. I will have to machine them this week or next. So I will use what I learned very soon. Thanks for your help! Jgaertner