Changing Tool Axis Orientation

[Digital_User]

Hey people,

I'm trying to machine the inner surface of the cylindrical workpiece, shown in the picture. The workpiece is a converted step file from a originally stl file of a 3D scan. It has no thickness and includes only triangular mesh elements. So it isn't possible to select a inner and outer surface of a triangular element. It's only possible to select the whole triangular element.

The problem is that Mastercam 2021 automatically machine the outer surface of the workpiece, as you see in the picture, when I choose the multiaxis parallel toolpath and select all the elements.

I already tried to import the workpiece with a rotation of 180°, so the inner surface is at the top. I also tried to change the WCS, the CPlane and the TPlann, but nothing worked.

Is there any option to force Mastercam 2021 to machine the inner surface, i. e. to invert the tool axis about 180°?

 

I would appreciate your help.

[JParis]

Sharing a file is usually the best way to get the best answer

[Chally72]

In Mastercam 2022, you can view and flip the surface normal direction of mesh entities, so that would make this a simple fix. In 2021, I'm not actually sure if there's any way to even view mesh normals. There are a few different ways we could still work around this and force the machining from the backside. If you can upload a file, I could provide an example. 

[crazy^millman]

Covert the MESH to surfaces and then use the surfaces to control the normal with. Verisurf has a 30 day free reverse trial for Mastercam and has has the ability to flip the mesh normals.

[Colin Gilchrist]

Don't drive the Mesh > create a section of a Cylinder (Simple Ruled Surface), "underneath" the mesh.

Use the cylindrical surface as the "drive surface", and use the Normal to control which side of the surface you are cutting on.

Then use a "Collision Control" strategy, and make that Mesh object the "check surface" or "compensation surface", depending on which particular Toolpath you are using.

A simple "parallel" or "Morph" would give you control over "how the tool moves across the "drive surface", and then you can use the "Retract Tool, Along Tool Axis" Collision Control, to keep the tool tangent to the Mesh, instead of the cylinder.

[GoetzInd]

+1 To Collins' Idea

[Digital_User]

On 8/14/2021 at 6:59 PM, Colin Gilchrist said:

Don't drive the Mesh > create a section of a Cylinder (Simple Ruled Surface), "underneath" the mesh.

Use the cylindrical surface as the "drive surface", and use the Normal to control which side of the surface you are cutting on.

Then use a "Collision Control" strategy, and make that Mesh object the "check surface" or "compensation surface", depending on which particular Toolpath you are using.

A simple "parallel" or "Morph" would give you control over "how the tool moves across the "drive surface", and then you can use the "Retract Tool, Along Tool Axis" Collision Control, to keep the tool tangent to the Mesh, instead of the cylinder.

Thank you all for your replies.

@Colin Gilchrist your idea is clever. But isn't there an easier way?

For instance, I have a simpler object like in the picture below.

There is only one triangular mesh element with no thickness, imported as a step file. There is only the option in Mastercam 2021 to select the whole element, when I choose a mill machine and the multiaxis parallel toolpath.

Why is Mastercam choosing especially this surface to machine the part? Is there any option to "say" Mastercam to machine the opposite surface of the part?

 

I would appreciate your help.

[Colin Gilchrist]

4 hours ago, Digital_User said:

Thank you all for your replies.

@Colin Gilchrist your idea is clever. But isn't there an easier way?

For instance, I have a simpler object like in the picture below.

There is only one triangular mesh element with no thickness, imported as a step file. There is only the option in Mastercam 2021 to select the whole element, when I choose a mill machine and the multiaxis parallel toolpath.

Why is Mastercam choosing especially this surface to machine the part? Is there any option to "say" Mastercam to machine the opposite surface of the part?

 

I would appreciate your help.

Did you happen to read Dylan's reply above:

"In Mastercam 2022, you can view and flip the surface normal direction of mesh entities, so that would make this a simple fix. In 2021, I'm not actually sure if there's any way to even view mesh normals."

So, if you are using Mastercam 2022, you have the ability to view and flip the "normal direction" of the Mesh.

The problem with any Mesh, is that it is made from a collection of Triangles. Each triangular facet is a simple "flat" surface. It is 3 vertex points, plus a "normal" direction vector (point).

I would guess that Mastercam assigns a "global normal direction" to a Mesh Entity. I say this because I haven't seen an option to "view or flip" the normal direction of an individual facet (triangle).

Mastercam has added new capabilities for machining Mesh geometry, especially the last 4 releases of Mastercam. That said; you are still much better off using Surface or Solid geometry. Mesh entities do not contain any "curvature data". The quality is limited by the size of the facets used to "mesh" the model. This is essentially a 'static tolerance'. Yes, there are now some tools for re-meshing and smoothing an existing Mesh, but it will never be as clean as working directly with Surface data.

If you find yourself working with a lot of scanned data, Verisurf, RapidForm, and GeoMagics are the best tools for developing clean surfaces from that Point Cloud data.

[Chally72]

Mesh entities do come in with a normal, even if you can't display it in earlier Mastercam versions.

Even if you can't flip the normal directions, you can still simply change your tool axis control method or tool plane to force the tool to come from the opposite side, just as you can with surfaces:

 

[Digital_User]

45 minutes ago, Chally72 said:

Mesh entities do come in with a normal, even if you can't display it in earlier Mastercam versions.

Even if you can't flip the normal directions, you can still simply change your tool axis control method or tool plane to force the tool to come from the opposite side, just as you can with surfaces:

 

Thank you all for your answers.

@Chally72 this is exactly what I'm searching for. Could you please explain how have you done this?

I've tried it for my own use case but it doesn't worked, as you can see in the following picture.

In the beginning of the sequence, the mill tool is in the correct plane (Left). But when the mill starts to machine the part, Mastercam is machine the wrong plane (Right). I added the Mastercam 2021 file and the part in the annex to make my problem more clear.

Thank you for your help.

2021-08-18_test_part_triangle.emcam

2021-08-16_test_part_triangle.stp

[crazy^millman]

33 minutes ago, Digital_User said:

Thank you all for your answers.

@Chally72 this is exactly what I'm searching for. Could you please explain how have you done this?

I've tried it for my own use case but it doesn't worked, as you can see in the following picture.

In the beginning of the sequence, the mill tool is in the correct plane (Left). But when the mill starts to machine the part, Mastercam is machine the wrong plane (Right). I added the Mastercam 2021 file and the part in the annex to make my problem more clear.

Thank you for your help.

2021-08-18_test_part_triangle.emcam

2021-08-16_test_part_triangle.stp

The start move in backplot is and seems always be part of Mastercam for every version is wrong. Unless the model and toolpath are at TOP/TOP/TOP you will alway see this false start. In 5 Axis machining I always teach customers to ignore that 1st move and watch the rest of the motion. Mastercam is not kinematic aware as a software it is World aware as a software. Since the kinematics of the machine are not part of the core system then the backplot is not aware either. It needs a point of reference to start and since it is written from a World TOP method for all calculations then that is where it needs to make it's reference from. Post the code and see what they code tells you then you will see what I am explaining to you here. Your main WCS is right, but your C-T Plane is left so move the STL to top and set your planes to top and backplot again and you will see the problem go away.

[Digital_User]

Hey everybody,

I've got the solution for my problem from my business partner.

There is an option to invert the normal of a surface. The result of this is that Mastercam will machine the inner surface of my cylindrical part.

Thank you all for your help.

All the best.