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Doing Splits the easy way: Splitting Surfaces in CATIA V5

By Scott Henderson

The Split command is an essential tool when working with surface-based models in the Generative Shape Design and Wireframe and Surface Design workbenches. It’ll let you take an existing surface that is a bit too long, then cut it down to the correct size and shape.

Doing a basic surface split is relatively straightforward. However, there are a few not-so-obvious choices and options in the Split dialog box. 

Split versus Trim

Before we start, there’s another tool that looks very similar to Split – both in appearance and functionality – and that is Trim. The main difference between these two commands is that Split is only cutting specific surfaces while Trim will cut all surfaces involved in the operation.

The Basic Split

A standard, two-surface split is relatively straightforward to build. Fire up the command, pick the surface that is to be cut down, then click the items that will be used to cut it.

In the image below, I want to cut the blue surface and use the yellow one to chop it down.

After clicking Split ( ), the dialog box opens and I’ve selected the Blue extrude as the element to cut and the Yellow Extrude as the cutting element.

Based on how we’ve selected items, we could see either of the results below. To swap back and forth between them, click the “Other side” button. The side that has the pale yellow, default surface color is the one that will be kept.

After that, a quick click of OK gives us the final result. Not too bad.

Multiple Cutting Surfaces

Next, let’s take a look at the same example, but now we want to make multiple cuts to the blue surface simultaneously.

The initial plan is the same: Fire up Split, select the item to be cut, then pick the cutting elements.

This time, it looks like only the area to the right of the purple surface will be kept.

One of the slightly confusing things about the “Other side” button is that it refers to the other side of the surface that is currently selected in the Split dialog box. So, in the above image, Purple Extrude.4 is selected, meaning we are picking the area to the right or left of that surface. We’ll potentially have to do the same thing for the other cutting elements, choosing to keep what’s in front or behind the Pink Extrude and what’s right or left of the Yellow Extrude.

An easier way?

Since that can be a bit of work, especially with a large number of cutting surfaces, here’s the easy approach: While selecting the surface to cut, choose the portion of it that you’d like to keep. A lot of times this will happen somewhat “automatically,” as we naturally choose the larger portion of the surface or instinctively pick what we want. Be deliberate about it, though, and you can guarantee you’ll get the correct portion of the surface.

In the image below, I clicked the surfaces, but didn’t really pay attention to where I was clicking. That led to getting the surface on the left as a result. To get the center of the blue surface, I’ll need to play around with the “Other side” options.

On the other hand, If I specifically choose the center of the blue surface first, then that’s what I’ll get, making the Split command much easier to use and saving a little time, too.

Multiple Cut Surfaces

In addition to using several surfaces to cut a part, it may be that several surfaces need to be cut. In this case, be sure to use the 'Selection Bag' icon to side of the list to select multiple items. The same selection rules apply here, too, so be sure to choose the exact portion of the surface you’d like to keep.

In the case below, I’ve built a new surface offset above the original surface. I’d like to split it, too.

After clicking the Selection Bag (  ), we can choose the choose the large middle area on the Blue Extrude and Blue Offset.

And, as a result, both surfaces are cut down to the correct size:

A word of warning with this one: The splits may be grouped together in the tree, which could have some organization and/or feature hierarchy implications later down the line.

To the Point

Here’s the quick version: Want to cut a single surface? Use Split. Don’t like playing around with the options in the Split menu? Choose the area of the surface you’d like to keep, then the Split command will do just that.

More Flexibility?

Of course, this is just a look at the basic options in the Split command. There are more options and settings buried below and we’ll take a look at those in future posts. Also, by using more complex base surfaces, the complexities of the split will be increased as well, leading to more challenging scenarios. Not to mention, we haven’t even touched curves yet.

In both the Introduction to Surface Design and Advanced Surface Design courses from Rand 3D, we go through an in-depth examination of the Split tools and practice using them in real-world scenarios.

 

CATIA V5 Tip: Sketcher Outputs

By Trisha West

 

Utilizing the four output commands within the sketcher workbench will allow sketch entities to be segmented individually, allowing for quick creation of shapes. In this video, trainer Trisha West, demonstrates the output feature, 3D Axis, 3D plane, and profile feature.

 

 

CATIA V5 Tip: Adding Balloon Callouts to an Assembly Drawing

By Trisha West

In this video, Technical Trainer Trisha West demonstrates how to add balloon callouts to an assembly drawing which requires generating the numbering convention, Bill of Material (BOM), and drawing balloons. Also included in this video is how to place the Bill of Material chart in the drawing using two methods: placing BOM in sheet background and also in the working view.

 

 

 

Creating a Manikin Simulation in CATIA V5

By Trisha West

 

In this video, Technical Trainer Trisha West shows the two methods of creating a manikin motion file: a simulation using saved manikin postures in a catalog, and creating a track with a manikin object.

 

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

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.

 

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