How to machine countersinks when they are already in the model?

[jgaertner]

Seems like I am always being challenged by countersinks. I have a part that was drawn with the countersinks

already in place. The part was drawn by my client in SolidWorks and sent to me. Is there anyway I can trick Fusion

into machining these countersinks? Please see attached picture.  Thanks. 

[seth.madore · Accepted solution]

Of course! You can use 2D Bore and select them, you can use 2D Contour, select the BOTTOM EDGE of the countersink and choose a chamfer tool, defining your chamfer size as zero and whatever offset you prefer

[jgaertner]

Thanks Seth,

I will give these suggestions a try and see whether I am able to pull this off. After 12 hours of machining the part, I am very hesitant to try something I am not sure about. May just do it manually on the old bridgeport! 

jgaertner 

[seth.madore]

You could always share the part here and we could toss some toolpaths on it 😉

Of course, I'm out of the shop now, so it might be a bit for a solution 

[CuttingEdgeManufacturing]

I usually just use the drill operation, and select a c'sink tool, and then make the bottom selection an offset from the hole top to the depth required.

i've never gotten around to doing it how seth has mentioned, with using a chamfer tool. but ive heard good results of it.

[Anonymous]

I just use the "Drill Operation" with my countersink tool selected to do this operation.... Set "Bottom Height" box to "Chamfer Width" and it will place the tool at the modeled chamfer point..... If you want to add or subtract depth to this position just edit the next line "Chamfer Width" to be a +/- value as you need it.

[jgaertner]

I used your suggestion for Contour tool path. The tool I have is .375" in diameter but of course my parts have numerous, different countersinks. So using the Drill Op would not work. Plus I do not have that many countersinks of different sizes. I wish I could get the tool tip offset a little better dialed in cause it seems like the tip of the tool is not really cutting the material. 

[Anonymous]

Hello all...

I am not following your reason for not using the "Drill" method .... When you select the vertical hole and not the chamfer making sure you have the "Chamfer Width" option tagged, the same size countersink will adjust to the correct Z position for each hole you have selected.... It looks at the model to determine the stop point..... Make sure you are using a "Chamfer Tool Type" and it is defined correctly to the actual tool you have in the spindle...... Are you not seeing this in your programming?  I do it this way all the time with great success..... Let me know if this works for you.

Regards, Brian

[seth.madore]

@Anonymous Yes, your way is perfectly acceptable if you have the proper size countersink. I was actually thinking that he just had a chamfer mill and was interpolating it. I based that reply on other posts @jgaertner has made in the past. Sorry for any confusion