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Introduction to Model Based Definition with Creo Parametric 7.0
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Understanding the MBD Process

The basic Model Based Definition (MBD) process can be summarized in five high-level steps:

  • Prepare for Annotations Utilize MBD start part, understand/create combined states, view orientations, feature groupings.

  • Create Annotations Create dimensions, notes, symbols, driving, and driven annotation elements.

  • Modify Annotations AE display, hyperlinks, display datums.

  • Complete Combination States Add AEs to AFs, add reference surfaces, appearance states.

  • Publish for TDP Creo View model, derivative model.

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Figure 1 - Creating a Combined State

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Figure 2 - Modifying Annotations

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Figure 3 - Completing Combination State

Prepare for Annotations

Figure

Figure 1 - Creating a Combined State

To efficiently create a Model Based Definition (MBD) model, an MBD start part should be available from your company. In addition to default datums, parameters, view orientations, and other start part information, the MBD start part contains your corporate MBD standards, including schema, combined states, notes, and layers.

Once the model geometry is created, you can access Creo Parametric Annotate mode to begin selecting and displaying the combined states created as part of the MBD start part. You also create any combined states as well as associated layer states, which you then synchronize to the combined states.

Annotating the model begins with a selection of features to be detailed, and a plan for the primary viewing orientations, text direction, and dimension layout.

Create Annotations

Create dimensions, datums, notes, surface finishes, and GTOL annotation elements on the model for the desired features in the proper combined state. Select various reference types as needed to indicate the endpoints of dimensions, notes, or other call-outs.

Modify Annotations

Figure

Figure 2 - Modifying Annotations

You can now modify the different annotation elements. Move annotations to position them better, or change their z-depth by moving them to a plane. You can do the following to modify annotation elements: Flip arrows and change arrowhead display as needed. Modify witness lines by trimming, creating jogs, breaking, and clipping them. Create any necessary datum targets, display specific datum axes and planes as needed in selected combination states, and add hyperlink notes to reference documentation or other information.

If it will be necessary to assign additional references to annotations for inspection purposes, create an annotation feature in the model tree footer for the corresponding combined state. You can then begin adding the annotation element to this annotation feature.

Complete Combination States

Figure

Figure 3 - Completing Combination State

For the given annotation elements, add the additional references as necessary to the annotation feature.

Review the combination states and add the necessary hyperlinks as required to switch between the site map and the other combination states.

Create and apply appearance states to highlight references as necessary.

Publish for TDP

As part of the Technical Data Package, or TDP, publish the completed MBD model from Creo Parametric to Creo View. In addition to the Creo View model, create the derivative model in the STEP AP 203 format.

Understanding the MBD Process

Objectives

After successfully completing this exercise, you will be able to:

  • Prepare a model for annotations.

  • Create annotations in a machined part model.

  • Modify annotations.

  • Complete the combination states.

You are a design engineer at Zulu Tech Corporation. Zulu Tech has adopted Model Based Definition (MBD), and you have been given the bar light clamp and are tasked with completing the MBD annotations. Zulu Tech had already put into place the MBD standards in the start part, which was used in the creation for this model.

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Erase Not Displayed

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Process\MBD

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BAR_LIGHT_CLAMP.PRT

Steps

  • Step 1. Prepare a model for annotations. Disable all Datum Display types. Figure For the purposes of this procedure, the model geometry has already been created, and the model is mostly annotated. In a real world scenario, you would create a new solid model using your company start part and then create the model’s features.

  • In the ribbon, select the Annotate tab to access Annotate mode.

  • Notice the detail tree now displays above the model tree, and the combined states display across the bottom of the graphics window. Figure The combined state tabs and names that display across the bottom are part of the MBD start part standards at Zulu Tech.

  • Select the 2_General combined state tab.

  • Notice all the notes and titles that are usually displayed in a drawing title block. Figure

  • Select the 3_Properties combined state tab.

  • Notice all the mass properties and material information. Figure

  • Select the 7A combined state tab.

  • Notice all the profile dimensions for the model. Figure

  • Select the 7B combined state tab.

  • Notice all the dimensions for the various holes. Figure

  • To create a new combined state, do the following: Click New Figure from the Combination States group.

  • Notice the newly created combined state all the way to the right of the other combination state tabs.

  • Right-click the Comb0001 tab and select Rename .

  • Type 7E as the name and press ENTER.

  • Drag to reorder the tab as shown.

Figure

  • To set the primary viewing orientation in the newly created combined state, do the following: Reorient the model approximately as shown.

  • Click Update Figure from the Combination States group.

Figure

  • Click View Manager Figure from the In Graphics toolbar. Select the Layers tab.

  • Notice the Layer States.

  • Click Close .

Figure

These layer states were created as part of the MBD standards in the MBD start part.

  • To verify the proper layer state was associated to the combined state, do the following: Right-click the 7E combined state tab and select Redefine .

  • Verify that 0_All_Off is selected in the Layers drop-down list.

  • Click OK .

Figure

The other layer states have already been associated to their corresponding combined states.

  • To set the active annotation orientation, do the following: In the ribbon, select TOP Figure from the Annotation Planes group.

Figure

  • Step 2. Create annotations in a machined part model. To create a driving dimension annotation element, do the following: Click Show Annotations Figure from the Manage Annotations group.

  • Select the Dimensions Tab Figure .

  • Select feature Extrude 7 from the model tree.

  • Select the R6 dimension from the graphics window.

  • Click OK .

  • Click in the background to de-select all geometry.

Figure

  • To create driven dimension annotation elements, do the following: Click Dimension Figure from the Annotations group.

  • In the Select Reference dialog box, select Select Surface Figure from the Select types drop-down menu.

  • Select the front surface.

  • Press CTRL and query-select the back surface.

Figure

  • Middle-click to place the dimension approximately as shown. Figure

  • To create another driven dimension annotation, do the following: Select the back surface of the slot.

  • Press CTRL and query-select the front surface of the slot.

Figure

  • Middle-click to place the dimension approximately as shown. Figure

  • Click Cancel from the Select Reference dialog box.

  • To create a note, do the following: In the ribbon, click FRONT Figure from the Annotation Planes group.

  • Select Leader Note Figure from the Note types drop-down menu in the Annotations group.

  • Select a location on the surface for the leader.

Figure

  • Middle-click to place the note. Figure

  • Type DO NOT ANODIZE .

  • Click in the background to complete the text entry.

  • Click in the background to complete the note.

  • To create a geometric tolerance annotation element, do the following: Click Geometric Tolerance Figure from the Annotations group.

  • Select the surface at location shown.

Figure

  • To place the geometric tolerance, do the following: Middle-click to place the geometric tolerance approximately.

Figure

  • To complete the geometric tolerance, do the following: In the Symbol group, click Geometric Characteristic and select Flatness Figure .

  • In the Tolerance & Datum group, delete datum feature symbol A , and press ENTER.

  • Delete datum feature symbol B and press ENTER.

  • Click in the graphics window background to de-select the completed geometric tolerance.

Figure

  • Step 3. Modify annotations. Zoom the model out if necessary so that the note and all dimensions display in the graphics window.

  • Click Update Figure from the Combination States group. Figure

  • To move the dimensions to a different plane, do the following: Press CTRL and select the 25 and 12 dimension.

  • Right-click and select Move to Plane Figure .

  • Select datum plane DTM3 from the model tree.

Figure

  • To move the 25 dimension, do the following: Select the 25 dimension.

  • Cursor over the dimension value and drag the dimension as shown.

Figure

  • To move the 12 dimension, do the following: Select the 12 dimension.

  • Cursor over the dimension value and drag the dimension as shown.

Figure

  • To flip the dimension arrows, do the following: With the 12 dimension still selected, click Flip Arrows Figure from the mini toolbar.

Figure

  • To modify the arrowhead, do the following: Select the note.

  • Cursor over the note arrow head, right-click, and select Arrow Style > Integral .

  • Click in the background to de-select the note.

Figure

  • Further move the dimensions as necessary. Figure

  • Step 4. Complete the combination states. To create an annotation feature, do the following: Click Annotation Feature Figure from the Annotation Features group.

  • Click OK from the Annotation Feature dialog box.

  • In the model tree, right-click the newly created Annotation 1 and select Move to footer .

  • Expand the Footer node.

  • Right-click Annotation 1 and select Rename Figure .

  • Type 7E as the name and press ENTER.

Figure

  • To add the annotation elements to annotation features, do the following: Select annotation feature 7E and click Edit Definition Figure from the mini toolbar.

  • Notice that there are no annotation elements in this annotation feature yet.

  • In the Annotation Feature dialog box, click Consume Existing Element Figure .

  • In the detail tree, select driven annotation element Note_45 .

  • Click OK > OK .

Figure

  • At the top of the model tree, click Settings Figure and select Tree Filters Figure .

  • In the Model Tree Items dialog box, select the Annotations check box and click OK .

  • Expand the Footer > 7E annotation feature.

  • Notice the associated note annotation element. Figure

  • To add a reference surface to an existing annotation feature, do the following: Select annotation feature 7E and click Edit Definition Figure .

  • In the Annotation Feature dialog box, select element AE_NOTE0 .

  • Press CTRL and query-select the two surface references.

  • Click OK from the Annotation Feature dialog box.

Figure

  • Expand the Footer > 7E annotation feature and select AE_NOTE0 .

  • Notice that the newly associated surfaces also highlight in the graphics window. Figure

  • Click in the background to de-select the annotation feature.

  • To add an appearance state that properly highlights the note references, do the following: Right-click the 7E combined state tab and select Redefine .

  • Select Note-Refs from the Appearance drop-down list.

  • Click OK .

Figure