You are here: Building a Process Model > Freeform Surface Machining Exercise

Freeform Surface Machining Exercise

Supported Applications: FreeForm Machining
Time Required: 15 - 30 minutes

This exercise will lead you through one example of using SmartCAM FreeForm Machining's surface machining processes to machine a part with freeform surfaces. In this exercise, you will load an ACIS SAT file of the part to be machined, then use SmartCAM's process modeling tools to generate the operations and toolpath needed to cut this part.

Concepts Explored

Step One: Load a CAD Model

Use File--New to start a new Process Model. Now, import the needed CAD model file.

  1. From the SmartCAM menu, choose File--Import.
  2. File Type: ACIS Text (*.sat).
  3. From File: Freeform_Solid.SAT. The SAT file is included with the other Learning SmartCAM model files. Use the File Selectbutton to help you find the file, if needed.
  4. Click on Accept to import the model file.

The model file is loaded. Press F12 to get an ISO view of the model. The imported CAD model looks like the following.


Step Two: Create a Material Boundary

A material boundary can be used for two purposes in this example. First it is used in the roughing operation to set the material boundary extents. Second, it is used by Show Cut to define shape and size of the displayed stock.

  1. Be default, SmartCAM starts a new process model with Layer geometry active. So, simply set the Layer number by entering 3 in the Insert Properties bar Step/Layer input box.
  2. Set the Level to 0.0 and Profile Top to 0.75. The Profile Top is set to the same height as the top of the part, this can be checked with Element Dataor using Utility--Measure.

The layer for the material boundary is created. Now, simply extract the material boundary from the solid model.

  1. Select Create--From Solid--Boundary to open the Boundary control panel.
  2. Create From: Surface.
  3. Surface: 17. This is the flat disc that is the bottom of the part. You can type in the value, pick the surface in the graphics view, or pick the surface in the Elements list view.
  4. Click on Create to create the boundary. The boundary is a circle that follows the circumference of the disc.

Step Three: Create needed Process Steps

In this example, this part will be machined with three different passes. First, a Roughing operation using a 0.25" End Mill, then a semi-finish pass using a 0.25" ball mill, and finally a finish pass using a 0.1" ball mill.

While each process step could be created as needed, for this example, you will create them at the same time.

Create roughing process step

Create a roughing process step using a 0.25" end mill.

  1. Select File--Planner to open the Job Operation Planner window.
  2. Make sure Process Step List is the active tab and press Add to create a new step.
  3. Add a Mill Roughing End Mill Process Step.

  4. On the Tool tab of the Edit Process Step window, set the Tool Diameter to 0.25.
  5. Press Update Desc to update the description.
  6. Switch to the Operation tab and set RPM to 1200.
  7. IPM: 40.
  8. Click on Update Desc to update the description.
  9. Click on Accept to add the process step to the process model.

Create a semi-finish process step

The next process step will be used for the semi-finish pass. It will use a 0.25" ball end mill.

  1. Select Add to create a new process step.
  2. Set Op Type to Finish Milling and Tool Type to Ball Mill.
  3. Tool Diameter: 0.25.
  4. Use Update Desc then switch to Operation tab.
  5. RPM: 900.
  6. IPM: 40.40
  7. Use Update Desc and then Accept.

Create a finish process step

The finish pass will use a 0.1" ball end mill.

  1. Add a new Finish - Ball Mill process step.
  2. Tool Diamter: 0.1.
  3. Update description and switch to the Operation tab.
  4. RPM: 1100 and IPM: 25.
  5. Update description and Accept.

The three process steps are added to the process model. Close the Job Operation Planner window.

Step Four: Create a Roughing Operation

A Surface Machining--Roughing operation will be used to create the roughing toolpath.

Select the step to use

Use the Insert Properties bar to select the step to use.

  1. Step the With Step/On Layer menu selection to With Step. Then set the step to 10.

  2. Set Level to 0.0, Profile Top to 0.75, and Clear to 1.0.

Create the roughing toolpath

Use the Roughing process operation to create the roughing toolpath.

  1. Select Process--Surface Mach--Roughing to open the Roughing control panel.
  2. On the Insert Properties bar, enable the Container button. When enabled, the generated toolpath will be stored in a single container element.
  3. The Roughing process uses surfaces in the active group as the part to rough. Enable the group arrow and select all surfaces on the solid. You can do this by double-clicking on any surface on the solid.
  4. Path Type: ZigZag with Cut Angle of 45.0.
  5. Stepover: 0.12.
  6. Depth of Cut: 0.2.
  7. First Pass Level: 0.75
  8. Finish Allow: 0.01
  9. Enable the material boundary, by checking the On check box.
  10. Boundary: 63. This is one of the elements of the material boundary created in Step Two.

  11. Press Go to generate the toolpath. When the process is complete, you will see the roughing toolpath in the graphics view and a new 65 Process container element in the Elements list view - this is the container holding the toolpath.

The generated roughing toolpath resembles the following.

Step Five: Create a Semi-finish Operation

The Project Pattern process operation will be used to create a spiral toolpath semi-finish operation. This operation will use Step 20 - the 0.25" Ball End Mill.

Hide previous created toolpath

So that it is easier to see what is being created, hide the just created roughing toolpath.

  1. If the Group toolbar is not already open, use the toggle button to open it. The button is on the Status bar, next to the Group arrow.
  2. Create a new Group, by removing all elements from the active group.
  3. Enable the Group Arrow and select the Roughing process toolpath. You can simply select any toolpath element or click on 65 Process in the Element list view. This will select all of the toolpath.
  4. Open the graphics view popup menu and select Hide Selected.

The previously created roughing toolpath is now hidden.

Select the step to use

Select the process step to use for the semi-finish process operation.

  1. Select 20:Fin Mill as the new step, on the Insert Properties Bar.
  2. Set Level to 0.0, Profile Top to 0.75, and Clear to 1.0.

Create the semi-finish toolpath

The semi-finish toolpath will use a spiral projection pattern.

  1. Select all surfaces on the solid by enabling the Group Arrow and double-clicking on the solid.
  2. Select Process--Surface Mach--Proj Pattern to open the Project Pattern control panel.
  3. Pattern Type: Spiral.
  4. Radius: 3. The entire part is 6" in diameter.
  5. Boundary: 63. From the material boundary created in Step Two.
  6. Wall Allowance: 0.01.
  7. Stepover: 0.1.
  8. Finish Allowance: 0.01.

  9. Click on Go to create the toolpath. When the process is complete you will see the new semi-finish spiral toolpath in the graphics view. Additionally, a new container named 66 Container is added to the Elements list view. This container holds the toolpath.

    If your Container button was not enabled, press Undo. Enable containers and then press Goto recreate the toolpath inside the container.

The semi-finish spiral toolpath looks like the following.

Step Six: Create the Finish Operation

The finishing operation will use the 0.1" Ball End Mill, Step 30, with the Contour surface machining process operation.

Hide previous created toolpath

So that it is easier to see what is being created, hide the just created semi-finish toolpath.

  1. Open the Group toolbar, if needed, and remove all elements from the active group.
  2. Enable the Group Arrow and select the Project Pattern container. You can simply select any toolpath element or click on 66 Container in the Element list view. This will select all of the toolpath.
  3. Open the graphics view popup menu and select Hide Selected.

The previously created semi-finish toolpath is now hidden.

Select the step to use

Select the process step to use for the semi-finish process operation.

  1. Select 30:Fin Mill as the new step, on the Insert Properties Bar.
  2. Set Level to 0.0, Profile Top to 0.75, and Clear to 1.0.

Create the finishing toolpath

The finishing toolpath will use the surface machining contour process tool.

  1. Select all surfaces on the solid by enabling the Group Arrow and double-clicking on the solid.
  2. Select Process--Surface Mach--Contour to open the Contour control panel.
  3. Pattern Type: ZigZag.
  4. Depth of Cut: 0.01.
  5. Enable First Pass Level and set to 0.75.
  6. Enable Final Pass Level and set to 0.1.
  7. Finish Allowance: 0.0.

  8. Click on Go to create the toolpath. When the process is complete you will see the new finishing toolpath in the graphics view. Additionally, a new container named 67 Process is added to the Elements list view. This container holds the toolpath.

    If your Container button was not enabled, press Undo. Enable containers and then press Go to recreate the toolpath inside the container.

The finishing toolpath looks like the following.

Step Seven: Verify toolpath

All the toolpath for this part is created. The next step is to verify that it correctly machines the part. You will use the Show Cut verification tool to handle this.

Adjust the view

Get a good, full ISO view of the part.

  1. Select View--View Orientation--Iso.
  2. Select View--Full.

Run Show Cut

  1. Select View--ShowCut to open the Show Cut dialog box.
  2. Stock Layer: 3. This is the boundary you extracted in Step Two. It will be used to describe the stock for Show Cut. After selecting Layer 3, a disc of stock will be drawn in the Show Cut window.
  3. Mode: Animate
  4. Optimize For: Quality
  5. Speed: 6. While Show Cut is running you can type a digit from 0 to 9 to adjust the speed.
  6. Click on Start to run the simulation.

The finished simulation will look like:

Tip
You can see all your generated toolpath by opening the graphics view popup menu and selecting Show Hidden.

Step Eight: Generate NC Code

The format of the NC code is controlled by the selected Machine and Template files. For this tutorial you will use pre-configured files that are shipped with SmartCAM.

  1. Select Process--Code
  2. Select a path and filename to store the NC code. You can enter the path directly into the "Code File:" input field or click File Select to display a File Open dialog.
  3. If the Machine= status shows <undefined> you will select the Machine and Template files.
  4. Enable: Show Path, Draw Elements, and Code.
  5. Set Speed: to 7.
  6. Click Start to generate the NC code.
    As NC code is generated, the related tool motion is shown and the generated NC code is displayed. When the simulation stops, the NC code is generated.
  7. Click Close to close the Code panel.

The NC code file is generated and stored at the path you provided. You can open it with any text editor. If you have installed Predator CNC Editor for SmartCAM, you can use the tool bar icon to launch the editor and load the code file.

Click the Predator icon on the tool bar.

Final Notes

This exercise showed one example of how SmartCAM is used for contour machining. But this is, by no means, the only method. There are many options and features available in SmartCAM and several different approaches could have been used to cut the same part.

The three mill toolpath operations were created with Containers enabled. This means, you can go back and experiment with changing the machining options to see what type of toolpath is generated.

Done

This exercise is complete.