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Creo Parametric Tip: A Design Consideration When Creating a Flat Pattern for a Complex Harness

By Natasha Reaves

 

This question was originally asked by a former student who attend the Creo Parametric Cable and Harness Design course and was answered by the class instructor. 

 

Student's Question:

What is the best method of creating a flat pattern for a complex harness? Even when I try manual, there is still a branch that won’t let me select it for a start point.

 

Instructor's Answer:

A possible solution to creating your flat harness linked to a complex assembly is to use a sub-harness.

In your harness part, you can create a sub-harness or sub-harnesses. A sub-harness is a portion of a harness (and not a separate part file); It is visible in the model tree in the harness Footer area. Using this you can possibly break up the wire features in “groups” that can be managed a little easier in the flattened harness model.

You can use all of the entities available for harnesses when working with sub-harnesses, but Creo allows you to also work with sub-harnesses separately in Harness Manufacturing mode.

(SIDENOTE: Harness-MFG module is used to create flattened harnesses from 3D harness parts).

To set the default sub-harness, use the MODIFY HARNESS icon located in the Harness group in Cabling mode. Then select the harness that includes the sub-harness you wish to set as the default. You can then click on Set Default and select the desired sub-harness.

 

More information about this topic can be found in our Creo Parametric Cable and Harness Design course.

 

 

Creo Parametric: An Overview of the Electromechanical Cabling Design Process

By Natasha Reaves

 

In the Creo Parametric Cable and Harness Design course, you will learn how to route electrical harnesses with and without schematic diagram information. Additionally, you will learn how to create flattened harnesses for manufacturing and how to document harness designs by creating flattened harness drawings that include BOM tables and wire list information.

In the Creo Schematics course, you will gain a full understanding of the schematic design process used to provide schematic data for the creation of electrical harness assemblies in Creo Parametric.

 

A process overview of the electromechanical cabling design process using Creo Parametric is shown below.

 

The following process outline describes how Creo Parametric is intended to be used to design electromechanical cabling systems.

1. Decide which cabling entities will be routed to various electromechanical devices in the assembly.

2. Using Creo Schematics, create a 2D schematic to represent the logical connectivity between the cabling entities and their respective electromechanical devices. 

3. In Cabling mode, create a realistic 3D assembly by routing cable geometry throughout the assembly. To expedite the design process, logical connectivity and parameters that are defined in Creo Schematics can be used in Cabling mode. In situations where it is not feasible to create a 2D schematic using Creo Schematics, other methods can be used to create a 3D cabling assembly using the logical reference method of defining cabling parameters and features.

Creo Parametric allows you to import logical reference information using the following files:

• Creo Schematics
• PTC Neutral file
• Mentor Graphics File

4. Using HARNESS-MFG mode, create a flattened harness to simulate laying out wire and cable harness geometry on a nail-board.

5. Create a 2D drawing to document the flattened harness for manufacturing. Use Pro/Report to create a customized bill of material and wire list. Drawings can also be created for the routed 3D assemblies.

 

More information about this topic can be found in our Creo Parametric Cable and Harness Design course and in the Creo Schematics course.

 

Creo Parametric Tip: A New Definition Option for the Datum Point Feature

By Natasha Reaves

 

In Creo Parametric a datum point can be used as a construction element when modeling geometry or as a known point for performing computations and model analyses. Datum points can be added to your model at any time, even while in the process of creating another feature.

 

A datum point feature can be a single feature or can contain multiple datum points that are created during the same operation. When multiple points are created in a single datum point feature the following apply:

• All datum points appear under one datum point feature in the Model Tree.

• All points in the datum point feature act as a group, so deleting a feature deletes all the points in that feature.

• To delete an individual point in the datum point feature, you must edit the definition of the datum point feature.

 

Creo Parametric supports three types of datum points that vary depending on their method of creation and use:

•   (Point) - A datum point created on an entity or at the intersection of entities, or offset from an entity.

•   (Offset Coordinate System) - A datum point created by offsetting from a selected coordinate system.

•   (Field) - A field point identifies a geometric domain and is used in Behavioral Modeling for analysis purposes.

 

To add datum points to your model, use the Datum Point feature tool located on the Model tab:

Or expand the area in the dashboard of the current operation and expand the point flyout.

Select the desired datum point creation tool.

 

Starting with Creo Parametric 5.0.2.0, a new constraint option is available to define a datum point feature. The new Project option can be used to project a datum point onto a planar surface, datum plane, or line.

The following images show the Datum Point dialog box with a selected vertex (left image), and then a selected plane (right image) that was needed to place the projected datum point.

 

 

More information about this topic can be found in our Creo Parametric Introduction to Solid Modeling, Creo Parametric Advanced Part Design, and Creo Parametric Behavioral Modeling courses.

 

Creo Parametric Tip: How to Add and Assign an Appearance to a Model

By Natasha Reaves

 

Creo Parametric allows you to customize the default system colors of parts and/or features. The Appearance Gallery is used to create, delete, modify, and save the appearance of parts and surfaces.

The Appearances icon    is located on the View tab under the Appearance group. Alternatively, you can access the Appearance Gallery palette using the (<CTRL + <SHIFT> + A) keys.

 

Below is an image of the default appearance gallery palette.

              

In Creo, you can define different appearance states for part and assembly models using the Appearance tab in the View Manager dialog box. With this functionality, you can define different appearance states and switch between the different appearance combinations for your designs.

 

Below are examples of the View Manager dialog box for part and assembly models.  

 

You can not change the Master Appearance. According to PTC, the purpose of the Master Appearance is to clear appearances. However, you can change the Default Appearance.

 

Use the following steps to change the Default Appearance:

1.  Open your model.

2.  Click on the    (View Manager) icon from the View tab or the In-Graphics toolbar.

3.  Click on the Appearance tab.

4.  Right-click on the Default Appearance and select Activate.

5.  Select     from the View tab.

6.  Select an appearance from the palette.

7.  Select the model, features, or surfaces on the model to change their appearance.

8.  Click      from the Select dialog box.

 

As stated earlier, you can define different appearance states for part and assembly models.

 

Use the following steps to create an appearance state:

1.  Open your model.

2.  Launch the View Manager dialog box by clicking on    (View Manager) from the View tab or the In-Graphics toolbar.

3.  Click on the Appearance tab.

4.  Click   .

5.  Enter a name for your appearance state.

6.  Select     from the View tab.

7.  Select an appearance from the palette.

8.  Select the model, features, or surfaces on the model to change their appearance.

9.  Repeat steps 4-8 for as many different combinations of colors, etc. that you need.

 

 

More information about this topic can be found in our Creo Parametric Introduction to Solid Modeling and Creo Parametric Advanced Part Design courses.

 

 

Rand 3D Webcast Working with Legacy Datums in Creo Parametric 4.0+ Questions and Answers

Thank you for attending my Creo Legacy Datums Webcast. If you missed the live webcast, you can view the recording here. https://resources.rand3d.com/creo-tips/rand-3d-webcast-working-with-legacy-datums-in-creo-parametric-4  

 

 

I had several questions asked during the webcast which I have answered below: 

Question 1: Is that "Create DFS option" new since Creo 5?

Answer to Question 1:

The Datum Feature Symbol command was introduced in Creo Parametric 4.0. In releases before Creo Parametric 4.0, a Set Datum was used.

 

Question 2: How many differences are there for Legacy Datums between Creo 3.0 and 4.0?

Answer to Question 2:

In Creo Parametric 3.0 (and earlier versions), a Set Datum was created as a property of a plane or axis feature. These referenced were either selected from existing references or created in the drawing.

In Creo Parametric 4.0 (and later versions), a Datum Feature Symbol is created as either a standalone annotation or inside of an annotation feature.

 

Question 3:

It appears you were able to add DFS to the model, why didn't you show annotations in the drawing?

Answer to Question 3:

Ideally, I would show the annotations in the drawing. What I wanted to demonstrate in the presentation is that you can add a datum feature symbol to the model or in the drawing.

 

Question 4:

If a DFS is created in Drawing mode, do they exist only in the drawing, or will it also exist in the model?  Does it matter which mode it's created in?

What are the impacts of not converting?

Answer to Question 4:

A DFS (datum feature symbol) created in Drawing mode exists only in the drawing; it will not exist in the model. If you want the flexibility of changing the references to affect both the model and the drawing, create the DFS in the model.

The impact of not converting to DFS in Creo 4.0 (and later versions) is that if you need to make changes to dimensions or geometric tolerances, you will first have to associate the dimension or geometric tolerance to model geometry, which is why we need to create a datum feature symbol. Also, the older method of using set datums is based off of outdated standards. You will be required to convert legacy datums to comply with the latest design standards.

 

Question 5:

In Creo 4.0 why would the rotate datum be grayed out?

Answer to Question 5:

If we are referring to the     button in the Additional Text group of the Datum Feature tab, you must enter text in the text field (make sure to hit <enter> key afterwards) in order for the button to highlight as shown.

 

Question 6:

How do you attach the DFS to a feature dimension in the model?

Answer to Question 6:

You just select the dimension to attach the DFS to. Once to select the dimension, you can move the frame to a desired location.

 

Question 7:

I'm new to Creo, why does it seem so difficult for such an easy operation?

Answer to Question 7:

A great question. I will say that as with most operations in Creo, there is a process. The process typically does not change much between versions. As the basic concepts are more important than the commands required to perform a task, in time you will be more comfortable with the process.

 

Question 8:

How do you get the dimension to show up?

Answer to Question 8:

I am not sure of the context, but you can show dimensions in the drawing using  Show Annotations option.

And you can display dimension in the model tree by selecting    (Settings) > Tree Filters > and check Annotations option. 

 

Question 9:

I think they was already stated but I wanted to confirm. If I am using an older drawing that uses ASME Y14.5 1994 per the drawing, will I have to use a CREO version prior to 4.0 in order to edit any of the datums or to create new GDT off of the legacy datums?

Answer to Question 9:

If you are using an older drawing that uses ASME Y14.5 1994 AND you need to edit this drawing in Creo 4.0 (or later version), you will need to open the model in the Creo 4.0 (or later version) and convert the existing set datums to datum feature symbol annotations. 

 

Question 10:

On a drawing I made recently, I got a duplicate datum name error.  But the way we do our drawings I need the ability to have datums A, B, and C in multiple parts shown on the same drawing in order for the tolerance notes to make sense.  Is that error message telling me that I have multiple datum C symbols on a particular part (which is something I don't want and thus is a useful error message) or is it warning me that I have multiple datum C symbols per drawing (and if that's the case is there a way to disable that warning?).

Answer to Question 10:

The following is the response from the attendee who asked the above question:

I figured out a work-around: by creating the DFS’s in the part instead of in the drawing (the key step I was missing was showing the dimension annotations in the part so that I could then select them when placing the DFS), I was able to create a separate datum C symbol on each part and then show them on the drawing annotations without it complaining.  So it does allow multiple datum C’s, one for each part, as desired.  My mistake was I expected incorrectly that when I created the datum feature symbol in the drawing attached to a part dimension that it would become a symbol associated with the part.  But it was associated with the drawing view, not the part, and thus CREO was somewhat justified in its complaint that I had two datum C’s because they were both tied to the drawing (in their respective views), not to the parts. 

 

Question 11:

In the newer style (Creo 4.0+), how are datum extension lines controlled/edited? They are currently displaying with a dashed line, and it needs to be a solid extension line.

Answer to Question 11:

Try setting the detail option leader_extension_font to SOLIDFONT.

 

Question 12:

Do the drawing mode options work if a combined state was used to create the drawing view?

Answer to Question 12:

Yes.

 

Question 13:

I do not see my draft datum created in the drawing in the model tree under annotations. I am using CREO 4.0 is there a specific way for the draft datum to appear the model tree on the part? Or does that only appear for legacy datums and not ones created in 4.0?

Answer to Question 13:

Draft datums do not appear in the model tree or in the part. In Creo Parametric 4.0, if the Annotate tab is active, draft datums will appear in the Drawing Tree under the Datums area (  ). If the Annotate tab is not active, you will not see annotations in the tree, though they are visible on the drawing.

If you want datums do not appear in the model tree, create the datum in the model. Then later when you are in the drawing, you will see that datum in the model tree. And you will be able to show the datum in the drawing using the   (Show Model Annotations) option.

 

Question 14: Can we step through an example of troubleshooting a set datum that is placed on a datum axis that is at an angle/normal to current orientation plane?

Answer to Question 14:

This question will be addressed in a future blog.

 

 

 

Creo Parametric Tip: Information About Bill of Materials (BOM) Report Formats

By Natasha Reaves

 

In Creo Parametric, the Bill of Materials (BOM) is a list of all the components needed to build the assembly. The BOM also lists the total quantity of each component included in the assembly.

To create a Bill of Materials, open or activate an assembly model, then click the  (Bill of Materials) icon. This tool is in the Investigate group on both the Model tab and the Tools tab.  Clicking on this tool launches the Bill of Materials (BOM) dialog box.

An example of the BOM dialog box is shown here.

Once you click     in the Bill of Materials (BOM) dialog box, Creo Parametric automatically saves the file with a .bom extension. This .bom file contains the bill of materials in plain text format and can be opened and viewed in a text editor, such as NotePad or WordPad.

The following image shows the message displayed in the status bar area of the user interface.

In Creo Parametric, the config.pro file is the configuration file that controls the environment settings. The configuration file option that sets the BOM format file to be used for a customized bill of material report is bom_format. You can view a Bill of Materials Report in the following formats: HTML output or text output. The default output format is HTML.

The BOM HTML format provides hyperlinks to each member and sub-member in the current assembly. It also provides hyperlinks that allow you to highlight, open, or obtain additional information about the models in the assembly.

The BOM text format lists the quantity, type, and name of each member and sub-member in the current assembly.

Also, you can set the info_output_format configuration option to either text or html. This option sets the default format type for information presentation. Setting text option will output the information as simple text. Setting HTML option will output the information as html data.

Additionally, you can set the info_output_mode configuration option to set the default method for presenting information. The options are both, choose, screen, and file. The both option allows you to view information on the screen and Creo writes the information to a file that you can view outside of Creo. The choose option allows you to manually select the method of viewing the information from the Menu Manager under the INFO OUTPUT menu. The screen option allows you to view the information on the screen only. The file option writes the information to a file only.

 

The following image shows an example assembly named top_level-assm.asm.

 

After clicking on Tools tab > Bill of Materials, the following two images show the bill of materials of top_level-assm.asm in both HTML format and text format, respectively.

 

 

As shown in both BOM Reports, the model top_level-assm.asm currently contains three components, component1.prt, component2.prt, and sub-assm1.asm. These BOM Reports also show that the component sub-assm1.asm contains two part models, component3.prt and component4.prt.

 

More information about this topic can be found in our Creo Parametric Introduction to Solid Modeling course.

 

 

Creo Parametric Tip: Information About the Drawing Setup File

By Natasha Reaves   

 

In Creo Parametric, the configuration file options control the design environment for parts and assemblies. This means that the configuration file, known as the config.pro file, is the master control file for the design environment.

The config.pro file can be accessed by selecting the File tab > Options > Configuration Editor.

An example of the Creo Parametric Options dialog box is shown here.

There is a specific file that controls the behavior of the drawing. This file is called the drawing setup file, and it has a .dtl extension.

The drawing setup file options add additional controls to the detailing environment. The drawing setup file options determine characteristics like the height of dimension and note text, text orientation, font properties, geometric tolerance standards, drafting standards, arrow style and lengths, and thread standards.

The drawing setup file can be accessed by selecting the File tab > Prepare > Drawing Properties and then click on the     command next to the Detail Options area. 

 

How To: Access and Edit the Drawing Setup File and its Options

1. Open your drawing file.

2. Click the File tab > Prepare > Drawing Properties. 

3. Click on  next to the Detail Options area.

4. An example of the launched Options dialog box is shown here.

5. Select or enter the required option in the Option area.

6. Set or enter the desired setting in the Value area. Default values are provided for the drawing setup file options, but Creo allows you to customize and save various versions for use in other drawings.

 

The drawing_setup_file configuration option allows you to specify the .dtl file that establishes the default drawing setup options for any drawing that you create during a Creo session. If you do not set this option, Creo uses the default drawing setup file option values.

 

More information about this topic can be found in our Creo Parametric Design Documentation and Detailing course.

 

 

Creating Creo Parametric Blends

By Trisha West

 

Technical Trainer, Trisha West, demonstrates the complexities behind the Creo Parametric blend function in this video including the importance of start point alignment and adding a blend vertex.

This topic is covered in the Rand 3D course, Creo Parametric: Introduction to Solid Modeling.

 

 

 

An Overview of the Capabilities of the Creo Behavioral Modeling Extension

By Natasha Reaves

 

The Behavioral Modeling module of Creo Parametric is also known as the Creo Behavioral Modeling Extension. This module is an optional advanced analysis and modeling tool.

Creo Behavioral Modeling Extension can be used to:

• Create geometry based on the results of measurements and other analyses.
• Check the feasibility of varying dimensions and parameters.
• Analyze parameter values as other parameters are varying.
• Optimize the model based on design rules and criteria.
• Study your design using several objectives.
• Graph the results of analyses.
• Create family table instances based on model mass properties.

By using the Creo Behavioral Modeling Extension, you can solve potential design problems, such as:

• Trial and error iteration of one or more design variables.
• Repetitive construction of a feature.
• Repetitive measurement of a feature.
• Feasibility and optimized solutions to a problem.

The Creo Behavioral Modeling module includes the following features and options:

• The datum analysis feature.
• The datum field point feature.
• Sensitivity Analyses.
• Optimization Studies.
• Feasibility Studies.
• Multi-Objective Design Studies.
• User Defined Analyses.
• Excel Analyses.
• Motion Analysis.
• Statistical Design Studies.
• Tolerance Analysis.

 

More information about this topic can be found in our Creo Parametric Behavioral Modeling and Creo Parametric Advanced Part Design courses.