Surface toolpath help

[Rakesh]

Hi every body

I created the draft surface which is 11 deg and .135" high and I have a ruled surface on the bottom of the wall which I can use as a checksurface. Now my problem is when I select the surface and select the cont0ur surface toolpath,the tool is going on the both side of the wall(mean going front and back face of the wall) I check the normal of the wall surface it looks ok. What I am doing wrong? If any any body can help

[rob@fain]

You may need to add a boundry to contain the tool

[Colin Gilchrist]

Under the Advanced Settings button, set the option to "only roll tool between surface(solid)faces". If that fails, you will need to create a 2D containment boundary and include it in your toolpath like Rob suggested.

 

HTH,

[crazy^millman]

You do need a boundary or check surface to keep this from happening. The contour toolpaths will always try to cut around the whole surface everytime unless boundary or check surfaces are used. Great toolpath just have to do a little work to use it verse Flowline which will do the same thing if you change it to one-way verse zig-zag. I use the flowline toolpath like this all the time in a one way direction to get plunging toolpaths for plunge milling.

 

HTH

[Colin Gilchrist]

You could also try Flowline if it is a single surface

[Guest CNC Apps Guy 1]

I'm with Colin, I'd go the Flowline route since it's a single surface you're cutting. More control over the toolpath, finish, etc...

[Rakesh]

With adding containment boundry it stop the tool going on the back of the face. Than I try the Colin suggestion of "only roll tool between surfaces", it also work even without giving boundry.

Thanks everybody who put the input.

Where I work we do mostly 2d machining so sorry for this type of simple questions.

Since I am on this surface topic I want to clear couple of more questions.

1. Is this not true when you select all the surfaces but the tool only go to those face which you can see on the top view

2.For draft walls,Flow line tool path gives better finish that Contour toolpath

If anybody can comments on these topics

thanks in advance

[Ron Branch @ Verisurf]

1: Think of it as looking down on the part the surfaces a tool can machine will be the ones that get machines.

 

2: Depends on a lot of factors I can get the same finish using both just depends on angle, surface, tool, adjacent surfaces, step over, and etc... You can make any toolpath make a good part just depends on how and to what extent you do it and use it to your advantage.

 

Also no question is simple if you do not know the answer to it.

 

HTH