CAM Studios

The components page will appear after creating a CAM Studio tab:

After adding a component to the CAM Studio, that component is added to the Components panel, and the Jobs panel is activated along with the Jobs toolbar.

툴바

The Jobs toolbar is activated upon adding a component to the CAM Studio and includes the following options:

(From left to right)

• Create job

• Create machine

• Create setup

• Create tool

• Create toolpath

Read specific details about each option in their corresponding sections below.

옵션 보기

The view options are located on the right side of the CAM Studio interface (shown below outlined in red):

The options available are:

Fit all	Center the visible models in the graphics area.
등각 투상	View models isometrically in the graphics area.
정면	Standard front-facing view of the models in the graphics area.
후면	Standard back-facing view of the models in the graphics area.
맨 위	Standard top-facing view of the models in the graphics area.
맨 아래	Standard bottom-facing view of the models in the graphics area.
왼쪽	Standard left-facing view of the models in the graphics area.
오른쪽	Standard right-facing view of the models in the graphics area.
Toggle transparency	Make the components or models in the graphics area transparent.

Click on a view icon to implement that view in the graphics area.

컨텍스트 메뉴

Right-click on a CAM Studio tab to access the context menu:

• Delete - Delete the current CAM Studio (even if it is active). The last remaining tab cannot be deleted.

• Open in new browser tab - Open this CAM Studio tab in a new browser.

• Rename - Rename this CAM Studio.

• Properties - Access the Properties dialog to provide more information about the CAM Studio.

• Duplicate - Make an immediate copy of the CAM Studio. Copies are pasted directly into the current document, automatically creating a new CAM Studio tab.

• Copy to clipboard - Copy the CAM Studio to your clipboard.

• 연결된 통합문서 업데이트 - 해당하는 경우 연결된 통합문서의 지정된 버전으로 업데이트할 수 있습니다.

• Move to document - Move the CAM Studio to a new or existing document. (If moving to a new document, the new document is created during this operation.)

• Create task - Create a task that can be assigned to another user (or the current user), that can reference a part and have a due date. Users specified in a task are notified of the task. You can create tasks from any Onshape CAM Studio, Part Studio, Assembly, and Drawing tab, and from the Tab manager context menu.

1. In the Components section, click the Add component icon to define the part for machining.

2. Select a Component type from the dropdown menu:

   

   Choose from these options:

   Part - The Component that will be machined.

   Workholding - Components that are used to hold the Part onto the machine. (This can include vices, soft jaws, hold down clamps, and more.)

   Stock - The raw material that will be machined away to produce the Part.

   A version reference is required for each of these options.

   1. Select a part. The part you select is added to the component list for machining, and the dialog closes automatically.

      

   2. Click Select item (under Component type) to open the Select part dialog.

Select the checkbox to the left of a component in the Component list to show or hide it in the graphics area.

Click the three dot menu to the right of a component to update linked document, open linked document, or delete that component.

1. Click Jobs (to the left of Components) to switch to the Jobs section.

2. Click the Create job icon at the top of the section (shown below with the tool tip underneath):

   

3. In the General section, enter a name for the job:

   

4. Expand the Bodies section, then select a part for the job in the graphics area.

5. Click Stock (to the right of Jobs) at the top of the section to access the Stock settings:

   

6. In the General section:

   1. Select a Stock type from the dropdown options.

      Box - Defines a bounding box around the target model. You can adjust the stock size with X, Y, and Z inputs.

      Cylinder - Creates a cylindrical stock model around the target part that can be adjusted.

      User defined - Allows you to designate a selected component that was designed in CAD and imported into the CAM Studio as the stock.

   2. Select a Stock direction type from the dropdown options:

      World - Selects the model origin for the direction type.

      Z and X - Selects Z and X axis points for the direction type. (Specify stock Z direction and stock X direction after selecting.)

      Z and Y - Selects Z and Y axis points for the direction type. (Specify stock Z direction and stock Y direction after selecting.)

      X and Y - Selects X and Y axis points for the direction type. (Specify stock X direction and stock Y direction after selecting.)

7. Expand the Dimensions section and enter the required parameters according to your preference.

8. Click OK to accept.

Click the three dot menu to the right of a job to edit, suppress, or delete that job.

1. In the Jobs section, click the Create machine icon (shown below with the tool tip underneath):

   

2. In the Machine section, the Group by machine manufacturer option is on by default. This option organizes the list of machines by manufacturer (as opposed to one long list, if the option is toggled off):

   

   An image of the Machine section with the Group by machine manufacturer option toggled on.

3. Click through each dropdown to select a machine that the part will be machined on.

4. In the Post settings section, edit the parameters for the post according to your preference. The settings are:

   Program - Select the output unit.

   NC general - Sequence numbering is toggled on by default. Enter a Block number start and a Block number increment. Optionally, toggle on the Block number at tools only or Block number as tool number options.

   Movement -Optionally, toggle off the default Rapid positioning option and manually enter a Rapid rate. You can also choose to toggle on/off the following options: Ouput Arcs, Arcs in XY plane, Arcs in XZ plane, Arcs in YZ plane, and Output helices. Enter the number of decimal places.

   Fixed cycles - Optionally, toggle on/off the following options: Drilling canned cycles, Peck drilling canned cycles, Thread tapping canned cycles, and Chip break canned cycles.

   A post, or post processor, is the translator used to convert the CAM data into Gcode for a specific machine controller type.

5. Click OK to accept.

Click the three dot menu to the right of a machine to edit then post, duplicate, or delete that machine.

The Setup establishes the Work Coordinate System (WCS) for job elements. Work coordinate systems are set reference points used to establish a known datum relative to the machine coordinate system. It defines the origin and orientation of the X, Y, and Z axes as they relate to the CNC machine, and it is the reference point for all machining operations. Multiple setups can be used.

1. In the Jobs section, click the Create setup icon (shown below with the tool tip underneath):

   

2. Fill in the parameters under the General and Position sections according to your preferences.

   Position Type establishes the Work Coordinate System position. Choose from:

   • World - Selects the model origin for the Work Coordinate System.

   • Component Box Point - Displays a bounding box around the component with selectable points to define the position.

   • Stock Box Point - Displays a bounding box around the stock with selectable points to define the position.

   Direction Type establishes the Work Coordinate System direction.

3. Click OK to accept.

Click the three dot menu to the right of a setup to edit, duplicate, suppress, or delete that setup.

1. In the Jobs section, click the Create tool icon (shown below with the tool tip underneath):

   

2. The Tool panel opens. In the Cutter section, optionally toggle the Library option on/off. While enabled, you are able to export the current tool library or import a new tool library into the CAM Studio using the import/export icons to the right of the Library toggle option. (Note, with the Library option toggled off, you are only able to import a new tool library and will have to manually enter parameters such as Machining type, Cutter type, Diameter, Cutter length, Overall length, and optionally toggle Center cutting on/off.)

   

   On the left, a screenshot of the Cutter section with the Library option enabled. On the right, a screenshot of the Cutter section with the Library option toggled off.

   The Machining type options are:

   • All - Displays all available tool types.

   • Milling - Displays all milling tool types:

     • Ball mill

     • End mill

     • Bull mill

     • Dove mill

     • Lollipop mill

     • Slot mill

     • Taper mill

     • Chamfer mill

   • Hole making - Displays all hole making tool types:

     • Drill

     • Thread tap tool

   Cutter type options and configurations vary depending on Machining type.

3. In the Tool panel under the Arbor section, optionally click Enable to use an Arbor to hold and secure the tool. While enabled, enter a name for the Arbor, select a Profile type, and optionally add point(s).

   

   Arbor defines the tool extension type.

4. In the Tool panel under the Holder section, Click Enable to use a Holder to secure the cutter. While enabled, enter a name for the Holder, select a Profile type, and optionally add or delete point(s).

   

5. In the Tool panel under the Assembly section, enter a number of assemblies.

   

6. Click OK to accept.

Click the three dot menu to the right of a tool to edit, duplicate, suppress, or delete that tool.

Arbor and Holder define a revolve with X and Z values. Their libraries allow the user to utilize one previously defined.

Importing tool libraries

To import a tool library:

1. Click the Import tool library icon in the Tool panel Cutter section (shown below outlined in red):

2. This opens the Select tool library dialog:

You can import directly from the current document, or browse Other documents to select from.

3. Optionally, click the Create version icon to create a version from the active document. Click the Version graph icon to see a version graph of the active document. Click the View released items icon (if applicable) to view the released items of that document.

Exporting tool libraries

To export a tool library:

1. Click the Export tool library icon in the Tool panel Cutter section (shown below outlined in red):

   

2. The tool library is exported into a new tab in the document.

3. Click the tab to access the tool library, where you can update or download the library.

1. In the Jobs section, click the Create toolpath icon on the right side of the section (shown below with the tool tip underneath):

   

2. The Toolpath settings section opens:

   

3. In the Toolpath Strategy settings section, fill in the parameters according to your preferences:

   Name - Enter a name for the toolpath.

   Type - Choose a type of toolpath from the options available:

   • Edges - Calculates toolpath based on wireframe input drive edges. It works without any machining faces.

   • Faces - Calculates toolpath based on input drive bodies.

   • Bodies -Calculates toolpath based on entire input bodies.

   • Holes - Calculates toolpath based on input holes.

   • Existing - Calculates toolpath based on existing operations.

   Pattern - Choose a pattern for the toolpath to follow from the options available:

   • 2-Axis rough - Used to remove large volumes of excess material quickly.

   • 2-Axis profile - Creates a toolpath based on the drive curves. (The drive curves will be flattened.)

   • 2-Axis chamfer - Creates a toolpath based on the drive curves and is used for chamfering and deburring operations.

   • 3-Axis profile - Creates a toolpath that follows the drive curves.

   • 5-Axis profile - Creates a toolpath that follows the drive curves where the tool axis is controlled by orientation lines along the drive curves.

   • Face - Used to machine flat areas. (The drive curves must be flat.)

   • Trochoidal - Provides sequential drive curve machining by trochoidal movements.

   • Engrave - Machines along the drive curves.

   Sub-pattern - Choose a sub-pattern for the toolpath from the options available:

   • Offset - Creates multiple cuts on multiple depths that will be offset from the selected machining surfaces.

   • Parallel - Creates parallel cuts on multiple depths.

   • Adaptive - Ensures that the cutting conditions remain almost constant. (This strategy avoids full-width cuts by constantly measuring the engagement volume of the tool with material and gradually removes material off of the remaining stock.

   1. Optionally, toggle the 2.5-Axis option which enables the machining of pockets and bosses.

   When examining toolpath information, all relevant parameters are presented for configuring the desired operation. As you adjust parameters, applicable options will filter out.

4. Fill in the remaining Toolpath Settings parameters according to your preferences:

   Offset - Specifies the amount of material to remain on the drive curves.

   Step down - Specifies the depth step.

   Step over - Defines how much the tool engages material horizontally for each pass.

   Sorting - Provides parameters for the Cutting method, Cutting directions, and Machined By.

   Heights - Set the Start height type, the Start height, the End height type, and the End height.

   Area - Set the Draft angle degree and (optionally) toggle the Close offsets option.

   Re-machining - Provides parameters for optimizing the toolpath to reduce cutting overages and only cut what is needed.

   Edge containment - Restricts the toolpath within the picked curves.

   Speeds - Define various toolpath rates and approaches. Set the speed for feed rate, plunge rate, and retract rate. Enable rapid approach, rapid retract, or adaptive feed rate.

   Posting - Defines the spindle speed and whether or not coolant is used during the machining process.

5. Click the Link section (to the right of the Toolpath section) to access the Toolpath Link settings. Fill out the parameters according to your preferences.

   Under the Clearance area dropdown section, Clearance area type designates the clearance area where the tool retracts to and approaches from for this operation.
   Under the First entry dropdown section, the Use ramps option determines if the tool utilizes the approach strategy or feeds directly into the material.
   The options in the Ramps dropdown section depend on the type of tool being used, the material being cut, and the machine rigidity.
   

6. Click the Axis section (to the right of the Link section) to access the Toolpath Axis settings. Choose an Output type, and (optionally) enable Tilting.

   When enabled, Tilting defines a tilt axis.

7. Click the Collision section (to the right of the Axis section) to access the Toolpath Collision settings. Fill in the parameters according to your preferences.

   The Collision groups dropdown section has the option to modify the toolpath with parameters for retracting, trimming and re-linking, and stopping the tool along a designated axis.

8. Click the Misc section (to the right of the Collision section) to access the Toolpath miscellaneous settings. Fill in the parameters according to your preferences:

   Profile pass - Adds a path to the toolpath that follows the profile of the drive curves.

   Smoothing - Optionally choose to toggle the following options:

   • Smooth corners - Creates fillets in the sharp corners of the toolpath. (Note that the fillets will not be applied to the outer contour of the toolpath.)

   • Smooth final pass - Creates fillets in the sharp corners of the outer contour of the toolpath.

   • Remove corner pegs - Automatically modifies the step over and adds extra cuts to the corners in order to remove the uncut material.

   Filtering - Choose to filter by Regions (removes the toolpath regions that are within the threshold value) or Contours (removes the toolpath contours that are within the threshold value). Choose a Filter type and enter a Filter threshold value.

   Quality - Enter a cut tolerance to specify the accuracy of the toolpath. It is the chordal deviation of the toolpath against the features to be machined.

9. Click OK to accept. The toolpath is added to the Jobs list.

Click the three dot menu to the right of a toolpath to edit, duplicate, suppress, or delete that toolpath.

Under the Jobs section, click the Preview operation icon to the right of an operation to view the Back plot, Verify, or Simulate. (To verify or simulate all operations at once, click the Preview operation to the right of a setup in the Jobs section.)

This activates the preview operation options in the bottom of the graphics area:

Each operation produces a different result:

Back plot - Moves the tool along the toolpath.

Use the top sliding bar to set the speed of the automation (the left side being the slowest, and the right side being the fastest).

Use the Step back, Run, Step next, and Cancel options as preferred.

The bottom sliding bar indicates the progress of the back plot animation.

Verify - Moves the tool along the toolpath while removing material, allowing you to find out more about gouges and excesses, and refine the in-process material (stock).

The sliding bar sets the speed of the animation (the left side being the slowest, and the right side being the fastest).

Use the Step back, Run, Step next, Go to end, Reset, and Cancel options as preferred.

Simulate - Previews the operation.

The sliding bar sets the speed of the animation (the left side being the slowest, and the right side being the fastest).

Use the Step back, Run, Step next, Go to end, Reset, and Cancel options as preferred.

The bottom row of buttons toggles the visual on and off for the tool, toolpath, workpiece, stock, and machine housing.

You also have the option to toggle pause on collision.