cad software

Quick Link

Suggestions

Happy CAMing: Machine Plastic Molds with Friendly New Features of ZW3D 2022

Full Story

Happy CAMing: Machine Plastic Molds with Friendly New Features of ZW3D 2022

ZWSchool 2021-07-27 19:50:00

CNC machining is for manufacturing objects like plastic mold cavities, cores, and sliders in the mold industry. The latest ZW3D 2022 contains more friendly CAM features to enhance the machining efficiency and experience. This article takes you through these features by the case of machining this plastic mold core.

Figure 1. The Plastic Mold Core

Machining this mold core mainly involves processes like roughing, semi-finishing and finishing. The operations include Offset 2D Roughing and Rest Roughing; Contour Cutting, Flat Finish, Lace Operation and Offset 3D Operation used for semi-finishing and finishing. Without further ado, download ZW3D 2022 and follow the steps below to practice!

Roughing  

Roughing includes Offset 2D Roughing and Rest Roughing, aiming to remove needless materials as fast as possible.

Offset 2D Roughing

It is a process that takes place in the first roughing. The following steps are an illustration.

Step 1: Insert Operation

In ZW3D, machining processes can be managed by files. The dimension of the material is 250*230*98, so we chose [D35R2] as the roughing tool.

Right-click on the folder named D35R2, select Insert Operation. Then, in the Operation Type dialog, select Offset 2D under the Quick Mill tab.

Figure 2. Selecting an Offset 2D Roughing operation

Step 2: Add Features and Select a Tool

Double-click on the Offset 2D Roughing operation, add the Part and Stock as features in the Primary menu, and select the tool [D35R2].

Figure 3. Adding machining features and selecting a tool

Step 3: Set Limiting Parameters

Set the Containment Type, the machining range in the Z axis direction in the Limiting menu, and the range of tool filters in the Filters menu.

Figure 4. Setting limiting parameters

Step 4: Set the Tolerance, Steps, and Toolpath

First, in the Tolerance and Steps menu, set the Tolerance and Thick and Stepdown parameters. Then, in the Path Setting menu, set the Flat Detection, Accuracy, and XY Corner Radius parameters.

It’s worth mentioning that the new Flat Detection function in ZW3D 2022 (as shown in the 5th step of Figure 5) spares you the effort of selecting each plane for inspection one by one when processing multi-layer planes, which is rather convenient.

Figure 5. Setting the Tolerance, Steps, and Toolpath

The Offset 2D Roughing toolpaths will be generated after the calculation completes. In ZW3D 2022, the multi-threaded parallel computing technology accelerates the toolpath calculation of Offset 2D Roughing significantly. What’s more, the Profile Roughing path pattern is available in Path Setting.

Figure 6. The Offset 2D Roughing toolpath and Profile Roughing path pattern

Rest Roughing

Rest Roughing aims to further remove needless stock more precisely for the subsequent Finishing process. Just like first Roughing, you could select the tool according to the shape of the part and the size of the previous tool. A tool whose radius is about that of the previous one is recommended (in this case, the D16R0.8 tool is selected).

In ZW3D the Rest Roughing typically uses [Reference Operation] to refer to the Offset 2D Roughing operation in roughing. After the corresponding tool is replaced, modify the Stepover and Stepdown parameters in Tolerance and Steps. Generally, specific parameters are set based on the tool radius and the engineer's personal experience.

Figure 7. Offset 2D Roughing process and Rest Roughing toolpaths

Semi-Finishing and Finishing

Semi-finishing is the process of preparing a workpiece for finishing by smoothing a few secondary surfaces to make its surfaces evenly thick. This will reduce tool wear during finishing, thereby improving the accuracy and smoothness of the workpiece.

As for finishing, it includes four processes: Contour Cutting, Flat Finishing, Lace Operation, and Offset 3D Cutting.

Contour Cutting  

Contour Cutting is the most-used method for high-speed machining and is usually done to machine the sides. High-speed machining takes the credit for high production efficiency, high processing quality, and low energy consumption. The following steps are an illustration.

Step 1: Insert Operation

The first tool used in Semi-Finishing is tool D16R0.8 according to the shape of the mold. Right-click on the folder named D16R0.8 and select Insert Operation. Select Z level under the Quick Mill tab in the Operation Type dialog.

Figure 8. Selecting an operation type

Step 2: Add Features and Select a Tool

Double-click on Z level, add the Part as a feature in Primary menu and select the D16R0.8 tool.

Figure 9. Adding a feature and selecting a tool

Step 3: Set Limiting Parameters

In the Limiting menu, set the machining range of Z axis and the filtering range of toolpaths in Filters.

Figure 10. Setting limiting parameters

Step 4: Set the Tolerance, Steps, and Toolpath

Set the corresponding Tolerance and Thick and Stepdown parameters in the Tolerance and Steps menu. You can set the corresponding XY Corner Radius and customize the cutting Start Points in the Path Setting menu.

Figure 11. Setting the Tolerance, Steps, and Toolpath

Step 5: Set Engage and Retract and Add a Link

In the Link and Lead and Link menus, set the Engage and Retract parameters and opt for Add Lead to Short Link.

Figure 12. Setting Engage and Retract and adding a Link

The Contour Cutting toolpaths would be generated after calculation.

Figure 13. Contour Cutting toolpaths

Flat Finishing

Used to machine the flat part surface, Flat Finishing can make the programming of the smooth surface more efficient and more reliable.

Step 1: Insert Operation

The D16R0.8 tool is also used here. Right-click on the folder named D16R0.8, select Insert Operation, and select Flat under the Quick Mill tab in the Operation Type dialog.

Figure 14. Selecting the Flat operation

Step 2: Add Features and Select a Tool

Double-click on Flat Finish, add the Part as the feature in the Primary menu, and select tool D16R0.8.

Figure.15 Adding a feature and selecting a tool

Step 3: Set the Tolerance, Steps, and Link and Lead

Set the corresponding Tolerance and Thick parameters in the Tolerance and Steps menu, as well as the Engage and Retract methods in the Link and Lead menu.

Figure 16. Setting the Tolerance, Steps, Engage and Retract

The Flat Finishing toolpaths would be generated after calculation.

Figure 17. Flat Finishing toolpaths

Lace Operation

Lace Operation is mostly used in machining flat areas to improve the accuracy and efficiency of surface machining.

Step 1: Insert Operation

So far, all surfaces have been machined by tool D16R0.8. With only a relatively small R angle (R0.5) left to process, the D8R4 tool should be used.

Right-click on the folder named D8R4, select Insert Operation, and select Lace under the Quick Mill tab in the Operation Type dialog.

Figure 18. Selecting Lace Operation

Step 2: Add Features and Select a Tool

Double-click on the Lace operation, add the parts and a new profile as features in the Primary menu, and select the tool D8R4.

Figure 19. Adding features and selecting a tool

Figure 20. Creating a new profile

Step 3: Set Limiting Parameters, Tolerance, and Steps

Set the Containment Type in the Limiting menu, then the corresponding Tolerance and Thick and Cutting Steps parameters in the Tolerance and Steps menu.

Figure 21. Setting Limiting parameters, Tolerance, and Steps

Step 4: Set the Cut Angle, Engage, and Retract

Set the Cut Angle in the Path Setting menu, then the Engage and Retract modes in the Link and Lead menu.

Figure 22.Setting Cut Angle, Engage, and Retract

The lace toolpaths will be generated after calculation.

It is notable that in ZW3D 2022, the sequence of lace operation has been optimized to make the ordering of the machining areas more reasonable and the cutting direction consistent, so that the generated toolpaths are of higher quality and safety.

Figure 23. Lace toolpaths

Offset 3D Cutting

Offset 3D Cutting is used to finish and clear corners of certain surfaces to achieve the required part quality and shape.

Step 1: Insert Operation

Since we’ve used the D8R4 tool before, choose D3R1.5 as a clear corner tool. Right-click on the Offset 3D Cutting operation under the folder named D3R1.5, select Insert Operation, and select Offset 3D under the Quick Mill tab in the Operation Type dialog.

Figure 24. Selecting the Offset 3D Operation

Step 2: Add Features and Select a Tool

Double-click on the Offset 3D Cutting operation, add the part and profile as features in the Primary menu, and select tool D3R1.5.

Figure 25. Adding features and selecting a tool

Step 3: Set Limiting Parameters, Tolerance, and Steps

Set the Reference Tool parameters under Limiting, then the corresponding Tolerance and Thick and Cutting Steps parameters in the Tolerance and Steps menu.

Figure 26. Setting Limiting Parameters, Tolerance, and Steps

Step 4: Set the Engage and Retract Parameters in Link and Lead

Figure 27. Setting the Engage and Retract parameters

The Offset 3D Cutting toolpaths would be generated after calculation.

Figure 28. Offset 3D Cutting toolpaths

Generate NC Codes

After generating all the mentioned toolpaths, output them as NC codes to start machining.

Step 1: Select the Machine

Double-click on Machine, click Post Configuration in the Machine Manager, select the corresponding post configuration controller from the list, and choose the [machine_all.mdf] as the definition file.

In ZW3D 2022, the NC codes of Siemens® and Heidenhain® CNC systems are supported.

Figure 29. Selecting the Post Configuration controller and Definition File

Step 2: Output the NC Codes

You could output all the NC codes for all the operations or an NC code for each tool.

Figure 30. Outputting NC codes

After that, the machine tool will machine the plastic mold core according to the NC codes.

Summary

The CAM module of ZW3D 2022 has been enhanced with functions such as the new Profile Roughing path pattern, Flat Detection, User-Defined Pre-Drilling points for Toolpath Generation, Siemens® and Heidenhain® CNC systems, and a 5-axis Head A on C machine. They can take your efficiency and experience in programming and machining to the next level.

Download the latest ZW3D 2022 for free and start your creation! Also, feel free to share your masterpiece with peer engineers in the Facebook ZW3D User Group.

For your better experience on our website and the display of relevant information, cookies will be used. Learn More