Chamfer error

[Roland12345]

I routinely break corners with a small radius to minimize deburring after machining. On this hex nut, if I use Fillet to put a .020 radius on the six corners of the hex and then try to put a .050 chamfer on the top edges, I get:

"Error: unable to construct Acis geometry for blend"

In the picture below, I substituted a .020 chamfer for the .020 radius and the .050 chamfer worked fine. Any idea why it won't work with the radius?

[rishivadher]

Hi Roland

That’s strange, just reproduce and dint gave me any error

I select all the part, and pressed “crt” to deselect which ones I don’t want to make the select radius

best Rishi

[AndrewSears]

The feature you are trying to create is not possible with Fusion.  Just to check I tried this with Inventor and the result is the same failure.

This is a modeling limitation we have where creating a chamfer larger than the radius will mean the shape manager building the CAD geometry would need to delete a modeling edge and create a new modeling edge.

Can you add this to the idea station?  

Thanks,

Andy 

[Roland12345]

Thank you Andy; will do. So is it technically possible to remove this limitation? I always put a small radius where two lines meet on an external mill profile like that so a bur isnt raised when the cutter rolls around the corner. I like being able to sit and watch the machining center run instead of scrambling to get the previous part deburred before the next one finishes. 

[Roland12345]

Thank you, Rishi - Andy was able to reproduce the error.

Roland

[rishivadher]

yep i realised that i dindt hunderud you question 🙂

[jakefowler]

Hi Roland,

Is this kind of result accurate/desirable? (with the chamfer driving straight through the fillets)

You can achieve this by modelling the large chamfer first, followed by the small fillets.

If you'd prefer the fillets to run-on to the chamfer (as it does in the chamfer-on-chamfer case), like this:

An alternative way to model this chamfer might be to use the Sweep tool; see the video below:

http://screencast.com/t/0vexbVpsaK8

Hope this helps!

Jake

[Roland12345]

Thank you Jake. Keep in mind that the .020 radius is strictly for bur prevention, and I'm approaching this from a machining perspective, having used 2D CAD/CAM for a long time. I'm accustomed to planning the machining operations without having a 3D model in front of me, and don't yet see all of this the way you veteran modellers do.

Typically the radius I use to break corners like this will be much smaller, more like .005 (large enough to prevent burs but small enough not to be noticed by a customer who did not intend to have a radius there). When I'm creating the toolpath for the chamfer cutter on this part, I would simply pick the same 2D boundary that was used to mill the hex profile in the first place, so the 45-degree chamfer cutter rolls around the corners the same way the end mill did. This is all very tiny, so maybe if I saw it under a microscope it wouldn't look like I think it would, but it works.

The problem I see with the examples above is that sharp corners now exist in the chamfer profile, which will introduce opportunities for burs to be created there. Climb milling will always push a bur out behind the cutter as it exits a sharp corner, and it gets worse as the cutter wears. A little radius here and there can save a lot of tedious deburring later.

In the picture below I created the chamfer first and then the .020 radius as you suggested. Then I also added a .020 radius to the corners of the chamfer path. This eliminates those sharp corners, but it doesn't match up with the radius on the hex walls.

This might be much ado about nothing, since I'm sure I can simply leave the chamfer off and deal with it in CAM (I haven't started learning that new program yet), but it would be nice to have the model accurately show the finished part. Also, if I want to machine a chamfer like this with a 3-axis operation and a ball end mill, instead of a 2-axis operation with a 45-degree cutter, I'll have to include the chamfer in the model.

[AndrewSears]

I am not sure if it is technically possible to remove this limitation within the program but I will ask and get a better answer for you.  We introduced the Idea Station for wish list or feature improvement suggestions from customers so please be sure to add this wish.

What Jake showed are the two ways we have to produce something similar.  I know those are not exactly what you want but if the features are so small that people will not notice then I hope those will work for you.

Andy

[Roland12345]

Thanks Andy. I'm participating in the CAM 360 preview too but haven't done much with it yet. I'm guessing that once I start actually programming some parts, a solution will be evident. I appreciate your help.