Rand 3D: Insights from Within

How to use formulas to construct geometry in CATIA

By Iouri Apanovitch

CATIA offers unparalleled capabilities for knowledge-based engineering. Parameters, formulas, design tables, etc. lie at the very foundation of CATIA, enabling capturing the design intent by creating relations among a model’s dimensions and features.

In this blog post, I will explain how to use formulas not just to link parameter values, but to create actual geometry in CATIA.

The Engineering Knowledge Language (EKL) used in CATIA’s formulas have a variety of constructor functions that enable building geometry using formulas or other types of relations such as Rules and Reactions. For example, there is a set of Circle Constructors for creating circles, Line Constructors for creating lines, Plane Constructors for creating planes, and so on. A snapshot of the Operations Constructors functions is shown below. As you can see, one can perform surfacing operations such as assemble, split, trim, and many others using those functions.

The function signatures as shown in the Members of list follow the same convention that is easy to learn. For example, consider the split function:

 split (tosplit:Surface, splitting:Surface, orientation: Boolean): Surface

The first word (split) is the name of the function. In the parentheses, you find the function’s input parameters. In this example, the first input parameter says tosplit:Surface, which means the function requires a surface as the first input, and the word tosplit implies that that would be the surface to split. The second input parameter says splitting:Surface, which means the function requires another surface as the input, and the word splitting implies that that would be the splitting element. The third input parameter says orientation:Boolean, which means the function requires either true or false as the third input, and the word orientation means that that would determine the side of the split to keep. Lastly, after the colon symbol you find the type of the value that the function returns. In this example, it says Surface, which means that the function’s result is a surface.

If you want to avoid guessing, look up the detailed descriptions for the functions in the CATIA’s Help system, in the Product Synthesis > Knowledge Advisor > Engineering Knowledge Language section.

As an example, I will use a formula to create an intersection curve between a plane and a surface shown below.

We start by creating a user parameter of type Curve. In the Knowledge toolbar, select the Formula icon. In the New Parameter of type pull-down list, select Curve, then click the New Parameter of type button.

Ensure that the created parameter Curve.1 is highlighted in the list of parameters and click the Add Formula button. 

In the Formula Editor dialog box that opens, select the Wireframe Constructors section in the Dictionary and double-click the intersect(Surface, Surface):Curve function in the Members of list, so it populates the right-hand side in the formula as shown below. Note that the space between the parentheses only contains a comma, which means we still need to select the two inputs to pass into the function.

To complete the formula, 1^st put the mouse cursor before the comma in the parentheses and double-click the plane in the tree, then, 2^nd, put the mouse cursor after the comma in the parentheses and double click the surface in the tree. The plane and the surface names now populate the space between the parentheses in the intersect function, as shown below.

Click OK twice to close the Formula Editor and the Formulas dialog boxes. The intersection curve displays in the model and in the tree as shown below.

The constructor functions in EKL could also be used to create geometry “on-the-fly”, without adding the created geometry to the tree and visualizing it in the model. For example, let’s say I only want to measure the area within the intersection curve, without actually adding the curve to the model.

Start by creating a new parameter, now of type Area. I will name it AreaIntersect. Then click the Add Formula button to open the Formula Editor.

In the Formula Editor dialog box, select the Measures section in the Dictionary, double-click the area(Curve,…):Area function in the Members of list, so it populates the right-hand side in the formula as shown below.

Select the Wireframe Constructors section in the Dictionary and double-click the intersect(Surface, Surface):Curve function in the Members of list. Now the formula should look as shown below.

Complete the formula by providing the two inputs for the intersect function, as I did in my previous example. The result should look as shown below. Note that due to the precedence rules (i.e. the expression in the parentheses is evaluated first), the intersect function is executed first, then its result is used as the input for the area function.

Close the Formula Editor and the Formulas dialog boxes. Note that the area parameter and its value are displayed in the tree, while the actual intersection curve is not. I.e. the intersection curve was computed “on-the-fly”, behind the scenes, and only used to calculate the area.

The use of parameters and formulas in CATIA is covered in the following Rand 3D classes:

• CATIA Introduction to Modeling
• CATIA Advanced Part Design
• CATIA Knowledge Advisor and Expert
  
  

How to use formulas to measure in CATIA

By Iouri Apanovitch

 

Any CATIA designer worth one's salt knows how to use Measure Item   
and Measure Between tools to make measurements. What is less known is that you can do the same using parameters and formulas, and this is what I will explain in this post.

The Engineering Knowledge Language (EKL) used in CATIA’s formulas has a rich set of measurement functions, located in the Measure and the Part Measures sections of the formula editor’s Dictionary, as shown below. For example, there is a distance function that lets you measure distance between any two objects, a length function for measuring length of a curve, an area function for measuring area of a surface or a closed curve, etc.

Although the function signatures as shown in the Members of list may initially seem cryptic, they all follow the same convention that is easy to learn. For example, consider this function:

                                                length (Curve, …): Length

The first word (length) is the name of the function. In the parentheses, you find the function’s input parameters. In this example, it says Curve, which means the function requires a curve as the input parameter. The “three dots” ellipsis symbol (…) means that the function can take any number of input parameters, i.e. that it could be used to measure the total length of several curves at once. Lastly, after the colon symbol you find the type of the value that the function returns. In this example, it says Length, which means that the function returns a value in length units.

You can look up the detailed descriptions for the functions in the CATIA’s Help system, in the Product Synthesis > Knowledge Advisor > Engineering Knowledge Language section.

 

Now let’s consider a couple of examples. In the first example, I will use a formula to measure the length of the spline shown below.

First, we create a user parameter that will hold the value of the measurement. In the Knowledge toolbar, select the Formula icon. In the New Parameter of type pull-down lists, select Length and Single Value, then click the New Parameter of type button.

Rename the created parameter from Length.1 to a meaningful name, such as SplineLength. To assign the measure value to the parameter, click the Add Formula button to open the Formula Editor dialog box.

In the Formula Editor dialog box, select the Measures section in the Dictionary list and double-click the length(Curve,…):Length function in the Members of list, so it populates the right-hand side in the formula. Note that the space between the parentheses is empty, which means we still need to select an input parameter to pass into the function.

To complete the formula, double-click in the tree the curve you want to measure, so it populates the space between the parentheses in the length function, as shown below.

Click OK twice to close the Formula Editor and the Formulas dialog boxes. The measurement and the formula are displayed in the tree as shown below.

In the second example, I will use a formula to measure the mass of the part shown below.

Similarly to the previous example, we start by creating a new parameter, now of type Mass. I will name it TotalMass. Then I click the Add Formula button to open the Formula Editor.

In the Formula Editor dialog box, select the PartMeasures section in the Dictionary, double-click the smartVolume(elem:Solid,…):Volume function in the Members of list, and double-click the PartBody in the tree to use it as the input parameter for the function.

Since mass is volume times the density of the material, we now need to add the material density to the formula. Add the multiplication operator “star” (*), click the material object in the tree, and double click the material density parameter in the Members of list. The completed formula looks as shown below.

Click OK twice to close the Formula Editor and the Formulas dialog boxes. The parameter and the formula are now displayed in the tree.

The use of parameters and formulas in CATIA is covered in the following Rand 3D classes:

• CATIA Introduction to Modeling
• CATIA Advanced Part Design
• CATIA Knowledge Advisor and Expert

Using Multiple-Value Parameters to control CATIA dimensions

By Iouri Apanovitch

 

In this post, I will explain how to control a CATIA dimension using a multiple-value parameter. As an example, I will use a sheet metal part shown below, in which the raw sheet material can only come in standard thicknesses, for instance, 1mm, 1.2mm, 1.5mm, and 2mm.

First, we will create a user parameter with multiple values. In the Knowledge toolbar, select the Formula icon. In the New Parameter of type pull-down lists, select Length and Multiple Values, then click the New Parameter of type button.

In the Value list dialog box, enter the standard thickness values, and click OK to return to the Formulas dialog box.

Rename the created parameter from Length.1 to a meaningful name, such as Thickness. Do not close the Formulas dialog box yet.

Next, we will link the sheet metal thickness to the created parameter.

Select the Sheet Metal Parameter.1 object in the tree. This puts the parameter view filter on the selected object, so now the list in the Formulas dialog box only displays the parameters for the selected object. Highlight the `Sheet Metal Parameter.1\Thickness’ parameter in the list and click the Add Formula button.

While in the Formula Editor dialog box, click the Thickness parameter in the tree, so it populates the right-hand side in the formula. This formula now equates the sheet thickness to the user parameter Thickness. Click OK to close the Formula Editor dialog box, then close the Formulas dialog box.

Double-click the Thickness parameter in the tree. Note than only standard thickness values are available for selection in the pull-down list.

Test the result by selecting different thickness values in the list and updating the part.

The list of standard thicknesses can be updated later, if necessary. To do that, double-click the parameter in the tree, then right-click in the value field, and select Multiple Values > Update Values in the contextual menu.

In the Value list dialog box that opens, edit the list as desired. In the example below, we’ve added standard thickness 1.8mm in between the 1.5mm and 2mm values.

The use of parameters and formulas in CATIA is covered in the following Rand 3D classes:

CATIA Introduction to Modeling
CATIA Advanced Part Design
CATIA Knowledge Advisor and Expert

CATIA V5-6 Tip: How to Customize Your Toolbars and Reset the Position of a Toolbar

By Natasha Reaves

 

There are many workbenches in CATIA. Each workbench has several toolbars available to suit your requirements and preferences. Depending on your monitor size and display resolution, your screen might not be able to display all the available toolbars. Fortunately, in CATIA you can customize the toolbars.

To launch a toolbar, select View tab > Toolbars, as shown:

The    next to the name of the toolbar indicates that the toolbar is launched. To remove a toolbar, select the    to clear the icon. Do not use the icon in the toolbar, because doing so may remove the toolbar entirely from the screen. 

 

To restore the original positions of a toolbar, select the Tools tab > Customize > Toolbars (tab) >   button, as shown: 

Each toolbar contains a separator ( ,  ). You can detach a toolbar from the application window by dragging its separator to a different location in the screen.

If more toolbars are launched than can be shown in the graphics window, double arrows appear at the corner of the screen, indicating that additional tools are available but are not visible.

An example image showing double arrows is shown here:

Either the separators or the double arrows can be used to reposition the toolbars on the screen.

 

 

More information about this topic can be found in our CATIA V5-6 Introduction to Modeling 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.

 

 

How to Overcome a Tricky Surface Offset in CATIA V5

By Scott Henderson

 

You’ve built your surface and the hard work is done. The shape looks good. Every bend radius is correct and all of the fillets finally mesh well. There’s just one last step: Thicken the part.

And now the real fun begins.

When it comes to solving problems, start with the easiest method first. If “easy mode” works and it takes care of the problem, you’re set. If not, no big deal – it only took a brief moment to try.

Part Design Thickness

If the ultimate goal is to get a thickened, solid part, head to Part Design and use the Thick Surface ( ) command from there.

For most simple and well-constructed surfaces, this’ll get the job done.

If it’s not going to work, we’ll know pretty soon by the error messages that’ll pop up.

If the offset value isn’t necessarily set in stone, sometimes a smaller number will allow the offset to be created. If that’s not possible, then we’ll need to find other solutions.

 

Generative Shape Design Offset

If Thick Surface doesn’t work, the usual next step is to head to Generative Shape Design and use the Offset ( ) function. There are extra options with this command that can help us out. 

If just switching commands is enough to offset the surface, then you’re almost done. Add some surfaces around the borders to close things off and you’re ready to go.

 

On the other hand, if the surface still can’t be offset, try playing with the smoothing options. These can allow the offset value to be imprecise, giving us a bit more leeway to create the surface. It looks like with this model, there are some areas in particular that just can’t be offset.

From here, we’ll have to do things the long way. The next move is to allow CATIA to skip any surfaces that it can’t offset. Typically, just by previewing the offset, CATIA will ask to remove the erroneous sub-elements.

The good news: There’s an offset! The bad news: The offset surface has a few holes in it and these gaps will need to be manually patched.

In this particular model, it looks like most of the surface has been offset pretty well. However, there’s an edge in the middle of the offset that’ll need to be cleaned up to help create a nicer surface later on.

We can use a spline and a split to remove the excess shape between two corner points, then Split the surface with the new spline to clean the edge. To ensure the spline sits directly on the surface, the “On Support” option is checked with the light blue surface selected.

With that done, it’s time to add Connect Curves. Ultimately, these’ll be boundaries for fill surfaces. The goal is to create a clean contour line for a smooth shape. Other wireframe tools can be used for similar results, too.

Once the curves are in, we’ll build three Fill Surfaces which will nicely finish off this offset.

To completely close the outside edges… you guessed it: more Fills.

We’ll add some Lines and Boundaries, then fill in the remaining openings at the edges of the model.

With that done, everything will be connected with a Join to create a final, singular surface.

Then as a very last step, we’ll head back to Part Design and fire up Close Surface ( ) to create a solid shape from the surface. Success!

Future Offsets

Of course, varying shapes will require different approaches. But, start with the easy options first, then dig into the complicated options if needed. Using Fills is a common approach to fix open gaps, but with all of the surface and wireframe tools in CATIA, there are a multitude of potential ways to tackle these issues.

If you find yourself needing more information about Splines, Connect Curves, Fills, Joins, etc., then the Rand 3D Introduction to Surface Design and and Advanced Surface Design classes are good resources. You can even find more info about the Close Surface and other surface/solid integration tools in there, too. Happy offsetting!