CAM Studios

1. In an Onshape document, click the Insert new tab icon in the bottom left of the interface.

2. Select Create CAM Studio from the menu. The new CAM Studio tab automatically opens.

You can utilize tool tips throughout the CAM Studio interface by clicking on question mark icons to read more information about various actions and options available.

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 on the left side of the interface.

Adding a component activates the Create job button in the toolbar at the top of the interface.

Toolbar

The toolbar is located on the left side of the interface, above the Jobs and Components panel, and includes the following options:

(From left to right) 

• Insert part, workholding, and stock

• Create job

• Create machine

• Create setup

• Create tool

• Create toolpath

• Create work plane

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

The toolbar buttons begin as inactive, and become active as you complete the steps in the CAM Studio process.

View options

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.
Isometric	View models isometrically in the graphics area.
Front	Standard front-facing view of the models in the graphics area.
Back	Standard back-facing view of the models in the graphics area.
Top	Standard top-facing view of the models in the graphics area.
Bottom	Standard bottom-facing view of the models in the graphics area.
Left	Standard left-facing view of the models in the graphics area.
Right	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.

Context menu

Right-click on a CAM Studio tab (at the bottom of the Onshape interface) 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.

• Update linked document - Allows you to update to a specified version of a linked document, if applicable.

• 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 on the left side of the interface, click the Insert icon dropdown and select a Component type to define the part for machining:

   

   Choose from these options:

   Insert part - The Component that will be machined.

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

   Insert 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 Insert dialog closes automatically.

      

Right-click on a component to access the context menu options: Edit, Suppress, or Delete.

1. Click the Create job button in the toolbar above the Jobs panel. The Create job dialog box opens: 

   

2. In the Job name field, enter a name for the job.

3. Click to activate the Bodies field, then select a part for the job in the graphics area.

4. In the Stock section, select a Stock type from the dropdown menu. Choose from:

   • 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.

5. In the Stock section again, select a Stock direction type from the dropdown menu. Choose from:

   • 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.) 

6. In the Dimensions section, manually enter the required parameters according to your preference.

7. Click to activate the Workholdings field, then select bodies for the job in the graphics area.

8. Click the green checkmark at the top of the dialog box to accept.

Right-click on a job to access the context menu options: Edit, Suppress, or Delete.

1. Click the Create machine button in the toolbar above the Jobs panel.

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. The Generic dropdown is open by default.

3. With Group by machine manufacturer toggled on, click through each dropdown to select a machine that the part will be machined on:

   • Generic

   • Bantam Tools

   • Brother

   • Haas

   • Hurco

   • Inventables

   • ShopBot

   • STEPCRAFT

   • Thermwood

   • Tormach

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

   • Program - Select the output unit.

   • Datum - Optionally, toggle off the default Advanced work planes option.

   • 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: Output 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.

Right-click on a machine to access the context menu options: Edit, Suppress, or Delete.

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. Click the Create setup button in the toolbar above the Jobs panel:

   

2. Fill in the parameters according to your preferences:

   • Component on machine

     • Name - Enter a name for the setup.

     • Program number - Enter a program number.

     • Machine mating - Select automatic or manual machine mating. If Manual is selected, manually enter the parameters for Offset X, Offset Y, and Offset Z. If Automatic is selected, the component will automatically move into an ideal mating position, considering the bottom area of the component mating with the machine connector. Machine mating is responsible for positioning the component (in linear terms) in machine space.

   • Initial work plane

     • Name - Enter a name for the work plane.

     • Work plane origin - Select a work plane origin; choose from World, Component box point, Stock box point, or Manual. Work plane origin is responsible for positioning the datum in the component.

     • Work plane orientation - Select a work plane orientation; choose from Z and X, Z and Y, or X and Y.

     • Override datum - Optionally, override the automatically assigned absolute work plane datum.

3. Click OK to accept.

Right-click on a setup to access the context menu options: Edit, Suppress, or Delete.

1. Click the Create tool icon in the toolbar above the Jobs panel.

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, Unit, Tool hand, Diameter, Cutting 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 cutter types.

   • Milling - Displays all milling cutter types:

     • Ball mill

     • End mill

     • Bull mill

     • Dove mill

     • Lollipop mill

     • Slot mill

     • Taper mill

     • Chamfer mill

   • Hole making - Displays all hole making cutter types:

     • Drill

     • Thread tap tool

   Set additional specifications for the remaining parameters:

   • Cutter type

   • Unit

   • Tool hand

   • Diameter

   • Thread direction - (only available for Thread tap tool Cutter types and is automatically synced with the Tool hand selection.)

   • Thread type - (only available for Thread tap tool Cutter types.)

   • Threads per inch - (only available for Thread tap tool Cutter types.)

   • Cutting length

   • Overall length

   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.

Right-click on a tool to access the context menu options: Edit, Suppress, or Delete.

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 Cutter section of the Tool panel (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. Click the Create toolpath icon in the toolbar above the Jobs panel.

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. (To choose the hole drilling order, use the Holes dropdown to enable the Select all blind holes and/or the Filter same diameter toggles.) 

   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:

   Drive edges - Select the edge or surface of a part to define where the toolpath should be cut. Choose Loop or Contour for the selection filter type. (Note that when a curve is inserted, the loop selection option cannot be used. You must select individual segments of the curve.)

   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.

Right-click on a toolpath to access the context menu options: Edit, Suppress, or Delete.

Work planes are coordinate systems that can be defined in CAM Studio, and serve purposes for both machining and output-NC.

1. Click the Create work plane icon in the toolbar above the Jobs panel.

2. In the Work plane section:

   

   • Name - Enter a name for the work plane.

   • Work plane origin - Select a work plane origin; choose from World, Component box point, Stock box point, or Manual.

   • Type - Select a type for the work plane to define a method of output for toolpaths in a given work plane. Choose from the following options: 

     • Absolute - The output is in a fixed datum pre-created (equally-defined) on the machine/control.

     • Dynamic - The output is in a temporary coordinate system, defined dynamically by functions such as "G68.2."

     • None - The output remains in the initial coordinate system (world), while machining/toolpaths stick to the defined work plane. (This typically does not involve transformation outputs in the generated NC.)

   • Override datum - Optionally, override the automatically assigned absolute work plane datum.

Right-click on a work plane to access the context menu options: Edit, Suppress, or Delete.

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 animation (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.

Export

To export an operation:

1. In the Jobs panel, right-click on the setup you wish to export to open the context menu, then click Post child operations:

   

   Click the Post selected operations option to export only the selected operations.

2. The Export dialog opens: 

   

3. Enter a program number as preferred.

4. Enter a file name as preferred.

5. View the selected machine model and post processor for the export.

6. Select a download option from the dropdown menu: Download, Download and store file in a new tab, or Store file in a new tab.

7. Click Export.