finish contour

[sml2011]

Hi

 

Can some one tell me:

in finish contour toolpath why the tool don't go down to the constant z of the bottom face? the tool is 0.01 up from bottom. why?

 

Is it for incremental depth cut?

I think we must always use absolute depth cut for finish contour?

 

 

Thank for for your consultation

[Colin Gilchrist]

Using Absolute or Incremental should not make a difference in the final position of the tool. Incremental is about where the geometry's Z height is.

 

Do you have "Stock to leave" set for the floor?

 

Also, when using depth cuts, Mastercam will calculate each rough depth pass automatically, but there is a separate value for finish pass on the floor. Are you looking at the path in Backplot? Where is your chain of geometry? Is it at the top of the contour, or the bottom of the contour? Check the depth of the geometry using Analyze Position.

[sml2011]

Using Absolute or Incremental should not make a difference in the final position of the tool. Incremental is about where the geometry's Z height is.

 

Do you have "Stock to leave" set for the floor?

 

Also, when using depth cuts, Mastercam will calculate each rough depth pass automatically, but there is a separate value for finish pass on the floor. Are you looking at the path in Backplot? Where is your chain of geometry? Is it at the top of the contour, or the bottom of the contour? Check the depth of the geometry using Analyze Position.

 

 

 

Hi daer colin

 

Yes you say true I check the back plot again i see that the tool go down to the constant z = -0.5 but i don't know why in the last back plot it show me z =-0.49

 

 

Can you please help me for parameters that i showed in attached picture.

 

 

 

Thank you

[Colin Gilchrist]

Ahhh, now I understand. You are using a Surface Finish Contour toolpath, I misunderstood and thought you were using a regular 2D Contour toolpath.

 

For a Surface Finish Contour Toolpath, The Cut Depths button is used to tell Mastercam where to start and end the toolpath in the Z Plane. Absolute and Incremental settings work differently, I'll try to explain them both.

 

Absolute uses Z depths that are related to your Z Origin point (based on the origin of your toolplane). You can enter values above or below the top of the surfaces for 'Minimum Depth'. The same thing applies to 'Maximum Depth'. When you enter a value for either of these parameters, you are referencing the Z origin of your Toolplane.

 

I will sometimes enter a value below the part in 'Maximum depth' when set to 'Absolute', to force Mastercam to create additional contour passes below the geometry.

 

For Incremental settings, the values work differently.

 

Incremental values are created directly off the surface or solid geometry.

 

-For Adjustment to top cut: A Positive value caused the tool to cut deeper in Z, relative to the top piece of geometry. A Negative value will move the tool up in the Z direction, away from the geometry.

 

-For Adjustment to other cuts: The options are reversed. A Positive value moves the tool away from surface vertically in Z, and a Negative value moves the tool closer to the surface.

 

Because this can be confusing (especially when you are first learning Mastercam), I usually recommend that people use 'Absolute' values.

 

The disadvantage to using the 'Absolute' settings is that you cannot just change the Origin values. If you need to change the origin position, then you must go into each surface toolpath that uses 'Absolute' values and change the numbers.

 

When you launch the 'Cut Depths' dialog box, press the Help button. You will get a help file that goes into much more detail about what all these buttons do. Also, in the help file, make sure you click on "Field Definitions" tab. This will give you a description of each parameter field.

 

Hope that helps,