New Mold Cavity Assembly

In this section, we will start the creation of a new Mold Cavity Assembly and we will review the main menus and icons.

Create a New Mold Cavity

Create a New file and then select the Manufacturing type and the Mold Cavity sub-type; You may uncheck the "Use default template" button to see the list of available template files.

If you have unchecked the "use default template", you are presented with the "New File Option" dialog box where you may browse to use your own template file, and where you may want to copy the associated drawings. In our example, we will use the default mmns_mfg_mold template. If there is a drawing associated with the template assembly file, then checking the "Copy associated drawings" will cause a drawing of your new mold cavity assembly to be started and saved to disk.

Press the OK button, and the Mold Assembly is created. If you press File > Save now, you will see that a .asm and a .mfg file have been saved to disk.

Understanding the UI

(Click on the image to enlarge it).

In this image, we notice several things:

- There is a PULL DIRECTION arrow pointing up: this indicates a default direction for the mold opening; This default direction is used by other features like parting line calculation.

- It is highly recommended to display the features in the model tree as most of the work will consist in creating features.

- The default features in this template model have been named to help the user to orient the model.

To change the PULL DIRECTION:

From the top menus, select Edit > Setup: the side menu manager appears,
Select PULL DIRECTION from the menu manager, and then select a most convenient reference for you (Plane, Curve, Edge, Axis or CSYS) to specify the mold Pull Direction.

From this point, the user is presented with top pull-down menus, right side menus (the menu manager), and special icons dedicated for the Mold Cavity environment. As a general guide, to create a new Mold Cavity Assembly, start from the top icon, and follow the icons down step by step.

Here is the list of Icons and the meaning of each one:

to assemble the design model (RefPart)

or to define the shrinkage of the RefPart

to create a Workpiece: the basic block that will be split

or to define parting geometry like sliders or core pins

to define a Parting Line around the RefPart

to create the Parting Surface(s)

or to split the Workpiece into several blocks

to create Pro/ENGINEER solid models out of the split pieces

to create a Mold Opening analysis

to trim the part where it intersects with the first or last selected surface of another part, quilt, or plane

to start the Mold Layout assembly application to create or modify a Mold Layout; you may prefer Pro/EMX automation to perform this operation.

The remainder of this tutorial will step through most of these icons.

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