Rand 3D: Insights from Within

CATIA V5 Visual Tip: Z-buffer Depth Display

By Trisha West

 

Here is another CATIA V5 visual option that some people find useful. By default, all reference features you create in CATIA will automatically “shine” through any other solid/surface leaving a cluttered screen.

You can change this option with the “Display all elements using Z-buffer depth." Once turned on, the reference items no longer shine through and you will only see them in their entirety if your camera is looking at it from the proper orientation.

 

CATIA V5 Tip: Low Light Mode in CATIA Assemblies

By Trisha West

 

In some CAD modeling packages, there is an automatic “tunnel vision” that occurs when you are active on a child component within a higher-level assembly. Below is an example of a CREO assembly, where a part file has been made active. Notice how the non-active files are ghosted out.

By default, CATIA does not have this option enabled, so when you activate on a component (in CATIA this is done with simply a double click), there is no visual change. To make this change, start by going into the CATIA internal option via Tools --> Options, then change the setting in the following location:

CATIA V5 Drafting Tip: Creating Detailed Views and Redefining Detail View Locations

By Trisha West

 

Creating a detail drawing view allows a user to enlarge areas within a drawing view to a different scale. In CATIA V5, you can select to make a detail view area in a circular shape, or a custom shape that the user creates.

First, let’s discuss the default option, Detail View.

Once completed, the area within the parent view will be circled and labeled.

And alternatively, the Detail View Profile.

Then, complete your drawing with dimension, notes, specialty symbols, etc. Here I have some dimensions calling out the depth of the hole details.

Sometimes, changes that you make to your drawing may require you to redefine the detail view area. Notice that both of my detail views are based on a section cut. Section cuts have a certain direction associated with them. In my case, the direction of the cross section shows the opening of the counter-drilled hole from the top surfaces. If I reverse the direction of my cross section cut, I have a problem.

Now if you are still creating the views and do not have any dimensions or specialty annotations in the detail views, then you can quickly delete the view and remake. However, if you already have annotations/dimensions in those detailed view, then how do you update the location.

First, you need to synchronize the view, then you can move the detail view areas.

Now we can redefine the location of the Detail View areas.

When finished, click on the “exit” icon.

Detail Views will now be updated. Any dimension/annotations will appear again attached to their parent reference.

 

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More information about this topic can be found in the Rand 3D training class, CATIA V5: Generative Drafting.

Updating Legacy Datums to Datum Feature Symbols in Creo Parametric 4.0+

By Scott Hendren

If you are new to Creo Parametric 4.0, and have started working with drawings or the Model Based Definition (MBD) annotation tools, you may be asking, “What is going on with Set Datums?” The simple answer is that Set Datums are replaced by Datum Feature Symbols.

In previous releases of Creo Parametric, a Set Datum was created as a property of a plane or axis feature. Now, a Datum Feature Symbol is created as either a standalone annotation, or inside of an annotation feature, and can only be placed on a surface, dimension, witness line, or GTOL.

In Creo Parametric 3.0 and earlier, Set Datum Tags could be created in one of two ways:

1. Using the (Set Datum Tag annotation) option in the Datum dialog box, as shown below, or the (Set Datum Tag annotation element) option from inside an annotation feature.
   
   
   
2. Using the (Set) option in the Datum dialog box.

   Prior to Creo Parametric 4.0, Set Datums were derived from existing datum planes or axes. Now, Datum Feature Symbols must be associated with model geometry. This means that when you open a model that was created in Creo Parametric 3.0 or earlier, you have to update any existing Set Datums to Datum Feature Symbols if you need to make any changes to dimensions, Geometric Tolerances, and so on. It is important to note that the Set Datums might also be connected to geometric tolerances, so you must manage that circumstance as well.

   As of Creo Parametric 4.0 M060, a Legacy Datum Annotations Conversion tool is available to help convert legacy datums to datum feature symbol annotations.

   The following steps should be followed:

   • Set the configuration option combined_state_type to mbd or semi_mbd. Note that Creo Parametric 5.0 uses semi_mbd by default.
   • Use the Model Tree Items dialog box to ensure Annotations display are enabled in the Model Tree, as shown below.

3. Right-click an annotation in the Detail Tree or Annotations group in the Model Tree and click Convert All, as shown below.

4.  In the ribbon, select the Annotate tab and click Annotations>Legacy Datum Annotations Conversion to open the Legacy Datum Annotations Conversion dialog box, as shown below.

Note the following:

• If you are working in Drawing mode, you must open the model and access the Legacy Datum Annotations Conversion dialog box from there.
• If you are working in Assembly mode, you must access the Legacy Datum Annotations Conversion dialog box from the top model.
• For annotations assigned from an inheritance feature, the Legacy Datum Annotations Conversion dialog box must be accessed from the source model.
  
  

5. All legacy Set Datums must be converted to Set Datum Tag annotations. Click Convert All Set Datums to complete that conversion. The results of the conversion appear in the Set Datums and Datum Annotations Table of the Legacy Datum Annotations Conversion dialog box, as shown below.

- If the conversion is successful, the datum is moved from the Set Datums column to the Annotations column and the Status column is empty.
- When a conflict is encountered, the datum is moved from the Set Datums column to the Annotations column, and displays in the Status column.
Change Reference appears in the Required Actions column.
- When a failure is encountered, the datum stays in the Set Datums column and displays in the Status column. Create DFS displays in the Required Actions column.
- You can hover over to see additional information related to a conflict or failure, as shown below.

6. Resolve the conversion conflicts by clicking Change Reference and selecting a reference on the model. The legacy Set Datum Tag annotation converts to a Datum Feature Symbol annotation. This must be repeated for all conflicts. Once corrected, the Annotations turn green, as shown below.


7.  When Creo Parametric cannot convert a legacy Set Datum, Create DFS displays in the Required Action column, indicating a failure. Several scenarios exist that could cause the failure, each requiring a you to edit the datum references:

• Scenario 1: A Set Datum is placed on a datum axis and the axis is normal to the current orientation plane.
• Scenario 2: A Set Datum is placed on a datum axis and the axis is at an angle to the current orientation plane.
• Scenario 3: A model Set Datum is placed on a Geometric Tolerance that was created in Drawing mode with the As Free Note placement type.
• Scenario 4: A model Set Datum is placed on a model Geometric Tolerance that was placed on a model dimension in Drawing mode. The dimension was created with the Dimension Elbow placement type and an Edge reference.
• Scenario 5: A model Set Datum is placed on a model Geometric Tolerance that was placed on a model leader note in Drawing mode. The note was placed with the Note Elbow placement type.
  
  

8.  Repeat the previous step for all the failures that have a workaround, and then click Convert All Set Datums to convert the legacy Set Datums to Set Datum Tag annotations.

9.  If no workaround (from Step 7) is available for the failure, click Create DFS to create a new Datum Feature Symbol annotation. The datum feature symbol annotation appears in green with the same name as the set datum. Repeat this step for all failures that do not otherwise have a workaround. Once complete, the Annotations display in green as shown below.


10. If any legacy Set Datum Tag annotations remain, click Convert All to DFS to convert all them to Datum Feature Symbol annotations, which will appear in green.

Note that you can use the Save Results option to save the current state of Set Datums and the Datum Annotations Table to an information file.

If you are working in a drawing, you have to open the part to perform the conversion operations. Once you have finished, return to the drawing and update all sheets using the following steps:

1. If there are multiple sheets, right-click a sheet and click Select All.
2. Select the Review tab and click Update Sheets from the Update This will update all of the drawing sheets.

Select the Annotate tab and click (Show Model Annotations) to display the new Datum Feature Symbols.

Using these steps you should be able to replace your legacy Datum Tags with Datum Feature Symbols to convert your older models to Creo Parametric 4.0.
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Learn more the creation and usage of Datum Feature Symbols and other model annotations in the Rand 3D Creo Parametric: Working with 3D Annotations and Model Based Definition guide. 

Creo Parametric Tip: How to use Pick From List to Select Entities

By Natasha Reaves

 

When using Creo Parametric, it is recommended that you review a list of all of the entities that can be queried based on where the cursor is located. One way to query items is to use the Next and Previous shortcut menu commands. Another way to query items is to use the Pick From List dialog box.

The Pick From List dialog box contains a list of items that are located directly under the cursor, even if the item is hidden. You can select a desired item from the Pick From List dialog box and continue designing your model.

Step 1.  Position the cursor directly over an entity.

Step 2.  Hold & press down the right mouse button; select Pick From List.

Step 3.  The Pick From List dialog box opens.

Watch as Natasha demonstrates the tip in this short video:

It is notable to mention that when you select an item from the Pick From List dialog box, Creo Parametric retains the highlighting of the selected item in the main graphics window when you spin, pan, or zoom the model.

 

Additional information about this and other selection methods are taught in our Creo Parametric Introduction to Solid Modeling course.

 

CATIA V5: Clash Analysis breakdown

By Trisha West

 

Performing a static clash in CATIA is a powerful tool that can detect areas of interference, contact and minimum clearance violations. In this video, we break down how to set up, read your clash analysis, and adjust internal setting for the clash in CATIA V5. Then we talk about two methods of visualizing the interference area with sectioning and Boolean operations.

 

 

More information about this topic can be found in the Rand 3D training class, DMU Navigator and Space Analysis.

 

CATIA Drafting Tip: Displaying View Axis in Drawing Views

By Trisha West

 

The default installation of CATIA V5 has the view axis displayed turned on in drawing views. This means that in the active view, there is a blue horizontal and vertical axis that is displayed and always aligned to the part’s origin location (or assembly). Depending on how a company designs their parts, this could mean that you have a part’s location far away from the part origin. This will cause your view frame is be overly large, which many (including myself) find annoying.

To turn this option off, simply find the option in your internal settings of CATIA using Tools --> Options to get started.

More information about this topic is found in the Rand 3D training class, CATIA Generative Drafting.