Navigation: How To ... >
How to Setup for Indexed Machining
VisualCAMc allows you to perform indexed machining with the use of multiple setups in both 4 Axis and 5 Axis mode. The Machine Definition tab of the Machine dialog controls the machine type and axis definitions. The Setup dialog controls the axis orientation specific for each setup. Here is the basic procedure and an example part.
This example part that requires indexed machining:
Indexed Machine Part
•What axis is your 4th rotational axis? This will be determined by the orientation of the Onshape part. In our example, the X Axis will be the rotational axis.
•Where will the Coordinate System Origin be? It must be on the rotational axis. You can define where using the Machine dialog.
1.From the VisualCAMc Toolbar select Mill and then select the Machine button or double left-click on Machine - 3 Axis under the Machining Job tree. The Machine defines the axis orientation of the machine tool you plan to use to machine this part.
2.Select the Machine Coordinate System tab.
3.By default, when the Machine dialog is displayed, the Machine Coordinate System (MCS) triad is aligned with the World Coordinate System (WCS) triad in Onshape.
4.Since the +X Axis will be our rotational axis, and the part is located in the +X direction, we do not need to change anything on this tab.
5.When you have verified that the MCS is aligned so that the Z axis (Blue) is pointing towards the top of the part, the positive +X Axis (Red) pointing toward the right and the Y Axis (Green) pointing toward the back, you can continue to the next step.
1.Select the Machine Definition tab of the dialog.
2.For Machine Type, select 4 Axis.
3.For the Configuration, select Table.
4.Check the box for Output all coordinate in local Setup Coordinate System.
5.Under the 4th Axis (Primary Axis) Parameters section, the Rotary Center should be set to 0,0,0. This is the location of the MCS relative to the WCS as is shown in the illustration above.
6.Now set the Rotary Axis to +X.
7.For Angle Limit, select No Limit.
8.Now pick Save to close the Machine dialog.
9.In the Machining Job tree you see that the Machine is now set to 4 Axis.
1.From the Machining Browser select the Post-processors tab or double left-click on Post - None under the Machining Job tree. The Post defines the Post-Processor that you plan to use when generating G-Code. VisualCAMc supports over 300 pre-defined Default Posts for the most popular CNC machine controllers.
2.The Default Posts are listed below the Posts in Document. You can select/drag a default post from the list up and drop it into the Post Processors folder of the Posts in Document. If you have a custom post you can use the Add Custom Post folder icon located on the toolbar to upload it to your Posts in Document folder.
3.Now select the Haas post and then switch back to the Machining Job tab. The Haas post is now listed in the Machining Job.
1.From the VisualCAMc toolbar select Mill and then Part Bounds Stock from the Stock menu. This will display the Part Bounds Stock dialog. The Bounds section of the dialog shows the size of the part as X: 8, Y: 3 and Z: 2.
2.If you want to add stock material in any axis, enter the amount of offset in the Offsets section of the dialog. For example, in the Machine Setup tab of the Machine dialog (mentioned above) we set the X Axis of the Rotation Center to -1.0 to move our part out further along the X Axis. You can add this to the stock vale also.
3.Pick Save to close the Part Bounds Stock dialog.
4.You will now see that Stock - Part Box Stock is listed in the Machining Job tree.
5. You should also see the Stock displayed around the part. If not, select the Toggle Stock Visibility icon from the display window to toggle the display of the stock.
The setup defines the orientation of the Machine Coordinate System for the toolpath operations under it in the Machining Job tree. When you load the Onshape part, there is a setup defined automatically, named Setup 1. Our part requires machining from two sides. This means that we need two unique setups, one to machine each side. You can create a new setup at any time. Since we know what they are, we will create them ahead of time.
Here are steps to define the Setups:
1.Double left-click on Setup 1 listed in the Machining Job tree to display the Setup dialog for that setup.
2.Change the name to: Setup 1 (Top).
3.From the display window make sure the Toggle Display of WCS triad is toggled on so that you can see both the MCS and the WCS triads. Note that the WCS triad is smaller than the MCS triad.
4.Verify that the MCS Z Axis (Blue) arrow is pointing towards the top of the part, in the same direction as the WCS Z Axis (Blue).
5.Pick OK to close the dialog. You will notice that Setup 1 (Top) is now listed in the Machining Job tree.
6.Now we will add Setup 2. First make sure Setup 1 (TOP) is selected from the Machining Job tree.
7.Then from the Mill toolbar select the Setup button. This will display the Setup dialog.
8.Change the name to: Setup 2 (Front).
9.Verify that the MCS Z Axis (Blue) is pointing towards the front side of the part, in the direction opposite the WCS Y Axis (Green). If it is not, set the Spin Angle to 90 and then select the X Axis, Y Axis or Z Axis buttons in the dialog until the MCS triad is aligned as shown.
10.Pick OK to close the dialog. You will notice that Setup 2 (Front) is now listed in the Machining Job tree.
A Work Zero is the machining program zero location, where all toolpath coordinates are calculated from. It is like moving the MCS to a location on your stock (or part) where you will be setting the program zero at on your CNC machine. In VisualCAMc you can define one or more Work Zeros under a setup. If no Work Zero is defined, toolpath coordinates are calculated from the MCS Setup location.
For this part we want define a Work Zero for Setup 1 (Top) and the Setup 2 (Front). The Work Zero will be set to -1.0 on the rotational X Axis.
Here are the steps to create the Work Zero(s):
1.Select Setup 1 (Top) from the Machining Job tree.
2.From the Mill toolbar select the Work Zero button. This will display the Work Zero dialog. Make these selections:
For Type, select Set to Stock Box
3.Now pick Save to close the dialog. You should see Work Zero listed under Setup 1 (Top) in the Machining Job Tree.
4.Now select Setup 2 (Front) from the Machining Job tree.
5.Again from the Mill toolbar select the Work Zero button. This will display the Work Zero dialog.
For Type, select Set to Stock Box.
6.Now pick Save to close the dialog.
7.You should see Work Zero listed under Setup 2 (Front) in the Machining Job tree.
8.Take a moment to select each Work Zero to confirm its locations relative to the stock or part as indicated in steps above.
9.Your indexed 4 Axis setups are completed.
Here are things to consider when creating and posting toolpaths in indexed 4 Axis mode:
1.When you create toolpath operations make sure they are located BELOW the Work Zero within the Setup that you are machining.
2.The rotation axis angle is posted as follows:
To perform indexed machining in 5 Axis mode, review the procedure above for 4 Axis mode and perform the following additional steps.
1.For your CNC Machine, determine the 4th (Primary) and 5th (Secondary) axis.
2.In the Machine Definition tab:
3.Set the Machine Type to 5 Axis.
4.Set the Configuration (Head-Head, Table-Head or Table-Table)
5.Set the 5th Axis (Secondary Axis) Parameters. including the Rotary Center, Rotary Axis and Angle Limit.
6.If the option Output all coordinates in local Setup Coordinate System is not checked, be sure to enter the Gage Length (for machines with a rotary head).