MillTracer Thread Data (Tab 1):

Import PointCloud (Back to top)

- Load an existing pointcloud file. This file contains all the coordinates to build any threadform and machine it with your selected milling tool.
A pointcloud for your spesific thread profile can only be made using ThreadTracer. Create a Pointcloud

There are included different pointclouds examples when you install MillTracer, you can import these from the PointCloud Examples folder.

[^] button (Back to top)

Eject a loaded pointcloud file.

Imported Point Data (Back to top)

This window shows basic information about the current loaded pointcloud.

AutoCS Faces (Back to top)

This button will create a new CS for every planar face thats selected on a solid.
If multiple planar faces is selected, it will create all the induvidual CS'es and select the last created CS as current.
If a single planar face is selected, it will create one new CS from the selected face, and set it as current CS.

Use Face Orgin- Checkbox
if checked it will create the new CS at the selected face origin (face become Z0 in the new CS)
If unchecked it will create new CSs at part origin.

Helix Parameters (Back to top)

Center X,Y,Z holds the start centerpoint of where the thread milling toolpath will be generated.

If using from a selected feature on a solid, these values will be automatically filled in with center coordinates from the solid feature.

If using a selected point, these values will be filled in with coordinates from the point.

If no solid is selected and no point is selected, the thread helixes will be generated from whatever values is set here.

Helix Construction (Back to top)

Helix Start Angle, is the angle around the centerpoint where the thread milling toolpath will start, use this to orient the toolpath around the centerpoint (X,Y).
To set the angle, just try some numbers (90,180,etc) and adjust based on how the geometry is drawn on your part. Any number between 0.000 and 359.999 will work.

Lead In Arc (Back to top)

Adds a Lead-in arc that the tool will follow before entering the material.

Always use a Lead-in Arc for Bottom Up milling, as the tool needs to properly feed into the material before starting the cut.

Lead Out Arc (Back to top)

Adds a Lead-out arc that the tool will follow out of the material.
The applied arc is adjusted to be equal to the thread height from the loaded pointcloud.

Always use a Lead-Out Arc for Top Down milling, as the tool needs to properly exit the material before going rapid to the next cut.

Thread Direction (Back to top)

Select to generate a righthand thread or a lefthand thread.

Milling Strategy (Back to top)

Top Down
Generate thread milling toolpath that starts at the top of the hole and ends at the bottom.


Bottom Up
Generate thread milling toolpath that starts from the bottom of the hole and moves up or out of the hole.
Bottom Up is preferable for thread milling right hand thread, as the tool will do climb milling.

When using points or manual coordinates, Start Z value will be where the tool starts, so for a Bottom Up thread, the Start Z should be the Z value in the bottom of the hole.

When a feature on a solid is selected, the Start Z value will be taken from the feature.
With Bottom Up selected, Start Z value will automatically be set to the bottom depth of the feature.
With Top Down selected, Start Z value will automatically be set to the top of the feature.

Override Pitch (Back to top)

When a pointcloud is loaded, the pitch of the thread is set here automatically. But you can set any thread pitch here.

The thread milling toolpath will be generated with the pitch set here, normally this should just be as is.

If the thread is a multistart thread, the pitch must be doubled for a 2 Start thread, and also use the Helix Start Angle to generate 2 sets of threads,
the second one with Helix Start Angle set 180 degrees opposite of the first set.

Thread Length (Back to top)

Length of the thread, only positive number here, the length is incremetal from the Start Z value.
If 'Top Down' is selected, the length will be incremetal from Start Z in the Z negative direction
If 'Bottom Up' is selected, the length will be incremetal from Start Z in the Z positive direction.

Visual Quality (Back to top)

Dropdown menu with 3 options, this is only for preview display when setting up the thread, as it only generates a visual toolpath.
Its fastest to use Single Helix option here during setup, and use this as a visual aid for adjusting X,Y,Z coordinates if needed.

Machine CS no. (Back to top)

Enter the CS to use. When generating thread milling toolpath, the CS selected here will be used.
When creating milling operations, the CS selected here will also be set as the machining CS.
Always doublecheck here that the correct CS is selected before enable Process Ops and clicking Do It

Roughing (Back to top)

Check to enable the roughing passes

Finishing (Back to top)

Check to enable the finishing passes
Leave both these checked to machine a complete thread with roughing and finishing passes.

Geometry Only (Back to top)

This is selected by default, used for setting up the thread, draws only geometry helixes.

Process Ops (Back to top)

Select when everything is set up, enable it and clicking Do It will generate the threading toolpath and create milling processes for the complete thread.

Do It (Back to top)

Do it button creates all the geometry and milling operations.

Creating a pointcloud in ThreadTracer (Back to top)

Pointclouds can be created using the internal post-processor in ThreadTracer.
First set up your thread profile in ThreadTracer, and use the tool parameters of the milling tool. Set stepdown and stepover cut depths that you want the milling tool to perform.


Select MillTracer Point Cloud in the dropdown menu, and enable NC PostProcessor

Enable Do Roughing and Do Finishing
Click Do It and a file requester will now ask for location and filename to save the pointcloud to your harddrive.

Import this file into MillTracer.





Page accessed : 365 times