Rand 3D: Insights from Within

Exporting 3D Annotations from CATIA to STEP

By Iouri Apanovitch

The Model-Based Definition (MBD), which deals with the definition of products through annotated 3D CAD models rather than traditional 2D drawings, is supported in CATIA by the Functional Tolerancing and Annotation (FT&A) workbench. The FT&A workbench enables the designers to embed the 3D Annotations, such as dimensions, GD&T symbols, etc., directly into CATIA 3D models, providing the ‘single source of truth’ for the manufacturing engineers and machinists.

Many large enterprises across the globe have adopted the MBD approach, so they no longer send 2D drawings to their suppliers. This presents a challenge for the suppliers, which is the ability to open and read the manufacturing information provided by their OEMs.

One obvious solution for the supplier would be to purchase CATIA software and use it to open and read the native CATIA models, including 3D Annotations. The problem for the smaller machine shops, however, could be the software cost.

Fortunately, there is another solution to this problem, which is using a neutral format such as STEP for data exchange. The STEP format has been around since 1994, but things have changed considerably with the advent of the STEP 242 protocol, which offers dedicated MBD support.

In this blog post, I will explain how to export CATIA’s 3D Annotations to a STEP file using the 242 protocol.

First, the pre-requisite is that you must have a proper license to be able to export, which is the SXT (Extended STEP Interface) add-on product. Having the ST1 (STEP Core Interface) license, included in most CATIA configurations, is not enough. Also note that the FTA (3D Functional Tolerancing & Annotation) license is not necessary. As you see below, I will be using the basic MD2 configuration along with the SXT license in my examples.

Second, you must activate some settings. Go to Tools > Options > Compatibility > STEP, activate the 3D annotations toggle, and select 242 ed1 in the Application Protocol pull-down list, as shown below.

Now let’s see how the export works for the part shown below.

Select File > Save As and select stp (*.stp) in the Save as type pull-down list. Click Save to save the STEP file.

Now open the saved STEP file in CATIA, as shown below. As you can see, the annotations came through just fine.

Note that the exported annotations are stored in the Annotation Set Result.1, which means they are not editable and cannot be deleted. However, the result annotations can be hidden if desired.

Things become a little trickier if you want to export an assembly with annotations, rather than a single part. As an example, let’s see how the export works on the product shown below, in which we have annotations on the product level as well as on the part level.

The export result is shown below. As you see, no annotations came through.

Turns out CATIA’s annotation export to STEP has some limitations, one of those being that the annotations on the product level cannot be exported. Specifically, this is what CATIA documentation says.

But what about annotations on the part level? To export those, you need to activate yet another option in the Tools > Options > Compatibility > STEP, which is Global nested assembly, instead of the default One STEP file.

Now the exported to STEP assembly opens as shown below. As you can see, the annotations on the part level have come through just fine.

 

The use of MBD and 3D Annotations is covered in the Rand 3D class: CATIA Functional Tolerancing & Annotation.

 

CATIA V5 Tip: Adding an offset to a Manikin Segment

By Trisha West

 

When performing a reach study on a human manikin, adding an offset is sometimes necessary to add when the manikin is using hand tools. In this video, see how to attach a tool, add an offset, and perform a reach study.

 

Executing a Manikin Hand Grasp in CATIA V5

By Trisha West

In this video, Technical Trainer Trisha West steps you through placing an object near the manikin, executing a manikin hand grasp and attaching the object to the manikin.

 

 

For more information including training classes that cover this topic, please contact us: [email protected] or visit our website: www.Rand3D.com 

 

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