How to machine using spherical cutter? 2

[sekhon]

Hello guys, Been trying to find a way to finish this part with a spherical tool but having problems.Nx 8.0 is not allowing the tool to touch the side walls of the part and sensing the shank would hit the top smaller opening of the part even thou shank is smaller than the tool dia.I am attaching 2 pics.One is of the part and second is the section view to better understand the part.Any help would be greatly appreciated. Thanks

 

[diamond3210]

What Drive Method are you using? If you are not using Surface Area try it. Use helical drive setting and Projection Vector set to Normal to Drive. Sometimes in Surface Area to do undercuts you may have to unpick the part and just drive the surfaces picked in Surface Area. Hope this helps.

 

[markrief]

This should be no problem with surface contouring.
Under Cutting Parameters, Clearances, check the Tool Neck clearance.

Mark Rief
Product Manager
Siemens PLM

 

[sekhon]

Thanks for the replies.I tried to generate a tool path using fixed_contour--->surface area and used zig zag. But the tool is moving up and down using zig-zag cut pattern.I got almost same results with helical cut pattern.and the tool is not machining the bottom face as i cant select the btm face.When i try to select the bottom face,it says cannot build grid.Is there any way,i can machine all the internal faces in a one shot using 3 axis mill? Normally i use fixed_contour with area milling while finishing cavities where no undercuts are involved. I am attaching the picture of generated path. Thanks

 

[diamond3210]

You have to specify the cut direction, in Surface Area click Cut Direction and pick the arrow that points the direction you want to travel, you may have to zoom in so that the arrows are not bunched together. To get the bottom surface you could make a 2nd operation for that surface alone using the same process.

 

[sekhon]

Hi diamond, thanks a lot.Yes it worked as i wanted.I changed the cut direction and used helical as u stated and it worked good.Could you please look into this(attached example).Its kinda same undercutting example.I want to machine shaded faces that are left by fixed_contour Area Milling but the problem is i am not able to select all shaded faces once using surface area.It says "cannot build grid". Any idea how can i accomplish this. Thanks again for your help.

 

[diamond3210]

Yeah that's a little more diffcult, the problem you're having with Surface Area is that in order to pick multiple surfaces they have basically to be four sided and the corners where they meet have to intersect within a certain tolerance that is set under Preferences, Selection, Chaining Tolerance. So short of building a sheet or sheets that encompass all of the surfaces using Through Curve Mesh, or N-Sided Surface that meet the Chaining Tolerance, I don't think that Surface Area is going to help here.

You could maybe try a Z-Level Profile op. with the Part selected and the surfaces selected for Cut Area and the cut levels set to scallop in Common Depth per Cut but I'm not familiar with the possibility of undercutting areas with this op. but if you can get this to work make sure in the Non Cutting Moves - Trim to Min. Clearance is checked with a specified Min. Clearance in the engages and retracts or else the cutter may violate the part on these.

I'm sure there is a better way of doing this, maybe someone else can chime in with a better approach.

 

[sekhon]

thanks diamond, Yes i have already tried z-level profile but it wouldn't cut undercuts.So definitely i need a different approach. Anybody Please.....

 

[markrief]

You can do it in surface contouring, but you need to create a drive surface and project sideways.
Before that, I would try Cavity Milling, profile cut pattern, turn off tolerant, turn on undercutting.

Mark Rief
Product Manager
Siemens PLM

 

[sekhon]

Thanks mark for the reply. I tried cavity milling but as soon as i uncheck tolerant machining,the option to specify cut area disappears while using workpiece as a geometry but if uncheck tolerant machining and use MCS Mill as a geometry and select just the shaded faces as a part,then the tool gouges into the workpiece.

 

[capnhook]

REALITY CHECK:

I guess what we have now is a lollipop cutter ----- THAT CAN"T DO ANYTHING.

Thanks for the lolipop cutters, I guess.....

Proud Member of the Reality-Based Community..

[green]To the Toolmaker, your nice little cartoon drawing of your glass looks cool, but your solid model sucks. Do you want me to fix it, or are you going to take all week to get it back to me so I can get some work done?[/green]

 

[diamond3210]

Thanks for the informative post, Capn. It must be nice having so little to do in life that you feel it necessary to troll all possible forums spitting out negative thoughts in every direction.

You have so much negative to say about NX lets see your software!

 

[capnhook]

Been using this software since the 1980's diamond3210. I know what I'm talking about......I have seen better CAM.

Keep on banging your head against the wall and don't complain, my friend. That's the kind of customer EVERYONE wants..!

Proud Member of the Reality-Based Community..

[green]To the Toolmaker, your nice little cartoon drawing of your glass looks cool, but your solid model sucks. Do you want me to fix it, or are you going to take all week to get it back to me so I can get some work done?[/green]