Step 1: Create the RefPart

In this section, we will show how to place the Reference Part (RefPart) and redefine its position.

Pick then select the model HUB_BOTTOM.PRT from the File Open Dialog.

You are prompted to decide if you want to keep working with the Same model or with a different but associated model (merge or inherited); it is up to you. Before making this choice, determine whether you may need to change the RefPart's geometry (note: applying a Shrinkage, for instance, will change the model).

It is highly recommended to work with an associative copy of the design model.

MERGE BY REFERENCE will create a model with no history or feature information,
INHERITED (our favorite choice) will create a one-way associative model where you will be able to access each feature and dimensions for modification, without changing anything to the original model.

For this tutorial, please select INHERITED and press OK; the new Reference Part named "MLD_HUB_BOTTOM_REF" will be created. This model belongs to the Mold MFG assembly and can be modified with no impact on the original model.

From here, you will notice that you have the possibility to assemble this model only once, or multiple times (you may test each option and hit PREVIEW to check the result):

SINGLE (our choice for this tutorial): the model is placed once in the assembly,
RECTANGULAR: will place the model as a pattern of parts with some user defined increment,
CIRCULAR: will place models on a circle pattern,
VARIABLE: will allow you to place any number of parts at any orientation/translation.

Important: the assembly of the model is done by aligning coordinate system to coordinate system; select the RefPart CSYS "CS0" and the Mold Assembly Origin "Mold_Def_Csys". You may change this at any time; you might be forced to change it if the part is not oriented such that the mold can be opened along the PULL_DIRECTION.

Press OK.

You are now prompted that the Assembly accuracy will be set to some value (taken from the reference model).

At any time, you may select the RefPArt that is placed now in the assembly and press "EDIT DEFINITION" from the RMB menu. If you do so, the same dialog box appears, but this time, you are not allowed to change the model, though you may redefine the placement as you wish.

To change the model, you will have to either delete the model and select a new one, or Edit > Replace... (or right mouse button (RMB) Replace) to replace the model with a different one.

Analysis

It is not too late to perform basic analysis of your model like Draft Checking or Slope... to check if the model is well positioned according to the Pull Direction or to start planning the sliders and other extra components that you may have to create to produce this part.

For instance, we will perform a Draft Check. Ther are two ways to access this:

Analysis > Geometry > Draft
- This is the standard Pro/ENGINEER tool,
- It will not use the PULL_DIRECTION by default.
- Select some surfaces and a pull direction. To select all the part surfaces, hover the mouse over one surface on the part (that is, pre-highlight a surface) and then RMB until "SolidGeom:..." is highlighted, then pick with the left mouse button.
Analysis > Mold Analysis and then select Draft Check from the TYPE drop down list
- Will use the PULL_DIRECTION by default,
- Select the Part and then compute.

You will prefer a 2 color analysis if you want to locate the "0" parting line,

You will prefer a 3 colors analysis with a draft angle set to some value (3 degrees here) to locate:

Blue: the surfaces from the "bottom" side,
Purple: the surfaces from the "top" side,
Yellow: the surfaces between +3 and -3 degrees (for instance).

You may want to zoom in on the details of the logo: this logo will require a slider to form it properly.

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