4 apr. 2017

Overview basic Analyse

When you enter a CAD program for the first time you will need to analyse coordinates, length, distances, angles, volumes and similar geometrical measurements.

This can be at a such early stage of your training, that you still have not been trained about the topic.Is that the case, you can use this overview to get a crash course in the most common analyse functions. In the WBT solution Grand Touring you find detailed description of all analyse functionality, if needed.

Analyse feature

When you analyse e.g: a distance between two faces, you will define an analyse feature, which will automatically be entered in the tree in a specific branch  "Measure".
If the design is modified, you can update the analyse feature and consultate the actual distance after the modification, without redefining the distance definition, which should be analysed.


The procedure by analysing and defining an analyse is in principle the following: (see also the detailed explanations afterwards.
  1. Selection of the analyse type
  2. Choose definition of the selected references
  3. Selection of the references
  4. Interpret the displayed result
  5. Decision to keep the analyse feature or not


If the geometry is modified and the analyse feature is influenced the tree entry is marked as not updated and the user can update it with the context menu.

Detailed Explanations

Type of analyse

The type of analyse is chosen by selecting an icon

A) Measure Between: distance and angle measuring....pair selection measuring
B) Measure Item:  coordinates, lengths, radius ...single selection measuring
C) Measure Inertia: volume, mass, main axis moments of inertia measuring

Defintion of the selected references

The interpretation of the selected geometry is chosen in a menu

Any geometry: The limits of the selected face are regarded as boundaries of the selected face.

Any geometry infinite: The limits of the selected face have no influences on the analyse. The face is looked upon as an unlimited plane.

Decision to keep or delete measurement

The defined analyse is kept by enabling the Keep measure option.


Content of Measurement

The analyzed parameter can be changed by selecting the button Customize. A panel will be opened in which desired parameters are selected.


26 mars 2017

PartBody versus Bodies

The CATpart file always includes a PartBody. It is there from the start and can not be deleted. The PartBody is a body, which is used as a container for a solid. In this sense the PartBody is identical to the other Bodies, which have been created with Insert > Body.

Meshing in PartBody

However the PartBody has a distinguishing mark. If the CATPart is going to be meshed due to a FEM computation, the program will automatically use the the solid in the PartBody. Therefore if you want to use a simplified solid geometry (A) for the meshing, the corresponding solid has to be placed in the PartBody.

Change PartBody

If you have designed the wrong geometry in the PartBody  it is easy to correct. Select the body you want to use as PartBody and then the context menu Body.# object > Change Part Body. The selected body will be changed into PartBody and the original one will transformed into a plain body. The PartBody will also be placed at the top of the bodies in the tree.

Buddy Thomas

25 mars 2017

Clean up from superfluous features

When you have completed the design of a part or reached a certain state you may want to clean up or in other words, erase superfluous features. This can be done by using the menu Tools>Delete Useless Elements. Before you execute this function, it is important, that you understand, what is looked upon as "Useless".

If you simply select the menu Tools>Delete Useless Elements and confirm the panel all features are erased, accept those who are parents to any solid features. All features, which have been referenced by creating a solid features are protected, from the bottom to the top of the Parent/Children chains. If axis systems are included in the file, they will then however be erased.
The elements, which are going to be deleted are highlighted in the list and in the geometry.


When you select the  menu Tools>Delete Useless Elements a panel is displayed and the result from the automatic scanning is presented. All elements (features/axis systems ...) are listed and there is an informative text, telling what will happen with the element, e.g. Keep solid, Keep, used by solid, Delete.
At the panel bottom a summary of the interaction is displayed, e.g.16elements: 4deleted 12kept. If you change the conditions the list and text are automatically updated.

Change the conditions

By using the context menu in the list, you can change the conditions. If an element has been assigned the operation delete in the list, the entry can be selected and thereafter the context menu Keep. This element will now be protected and also all its parents.


The surface has been designed and it shall be kept with all its parents and the second axis system. There is no existing solid feature.

  1. The menu is selected Tools>Delete Useless Elements
  2. The final surface feature is selected with the context menu Keep
  3. The second axis system is selected with the context menu Keep
  4. The summary is checked before the panel confirmation
Useful Greetings

19 mars 2017

Multi Selection by Hide and Show

In Catia Version4 there was a very often used function called "Multi Selection". With it a certain type of features, e.g. points, lines or planes could be accessed as a whole by entering an abbreviation such as *PT for points , *LN for lines or *PLN  for planes. This was done to hide or show and even delete features as an entity type in the model. A similar function is offered to show and hide features/sets/bodies/volumes in Catia Version5 not however to delete them.

Multi Selection in V5s in

Access all objects of the same type

Under the menue Tools>Show / Hide are a list of differrent objects gathered among them points, lines, planes, geometrical sets to just mention some. If a certain type is selected are all objects of the selected type processed showed or hidden.

The function includes all of the selected type and after the use all objects are either shown or hidden. A pity for example if you have put certain important planes in show and other planes of minor interest in hide mode. This seperation has then been lost.

Multi Success!

Overview Creating Images in Catia

Frequently I get the question how to create an image from the design in the CATPart or the CATProduct. For some unknown reason the corressponding functionality has been neglected during the training. There are also a lot of questions about settings and image file types. Therefore let us take a look at the issue.


Image Functionality in Catia

You find the function to create pixel and vector images under the menue Tools>Image>Capture. After you have had  created images, you can look and organize them with the menue Tools>Album.



When you create an image in Catia you define a rectangle frame. The part of the geometry and the specification tree inside the frame will be included in the image but not any opened panels or visualization of functionality symbols. If you need this kind of images, e.g. to describe the way to use Catia, you will need another software.
A possibility would be to start a Window product, for example PowerPoint and use Insert>Screenshoot and execute an image in the application Catia. After the execution you can copy & paste the image where you want to.
An excellent software to create images is SnagIt, which offers powerful qualified options. We can recommend it.



To execute an image you procede as follow:

  1. Zoom in and pan the geometry as needed
  2. Select the Menue Tools>Image>Capture. The capture panel will appear.
  3. Select file type icon, pixel (A) or vector (B)
  4. Select the Arrow icon
  5. Define the rectangle frame
  6. Select the Capture icon  (red spot)



The image is executed and appears after some seconds in the panel Capture Preview. You can now erase, save, print and copy the image.
Attention: To be able to continue with another image, you have to erase the active image from the panel. Click the first icon (the red cross).




Pixel or Vector Image

You can choose  between pixel and vector images.This is done by selecting one of the icons at the right in the Capture panel.

A pixel image is a defintion based on small spots. The accuracy is defined by resolution for example 72 dpi. This means that if you increase the size of the image it will appear less accurate. As a guideline newspapers have normally 150 dpi and high quality  books images have 300 dpi. For the web resolutions around 100 dpi are common.

A vector image uses all wireframe elements of the geometry and computes the corresponding vectors. These images are scaleable without any quality losses but visualizate only the wireframe and not the shaded faces of the parts.



Pixel File Formats

When the image is saved a great number of file types are offered, e.g.:
  • *.bmp      windows bitmap file type adopted to Windows products, small file size but also poor quality by shaded faces
  • *.jpg        adopted to photos and gives a good result by shaded faces
  • *.tif          high performance images but with big file size

8 mars 2017

Origin in CATPart a brief overview

Among the first things you have to consider starting the design of a new part, is where to place the origin. In the early releases of Catia V5 there were no coordinate systems and the origin was only represented by the three baseplanes xy, yz and xz. Under the pressure from especially the car producers Catia V5 also become coordinate systems. They are crucial for this industry.

Two types

If we look as an example at the components of a car, you have two types of parts regarding positioning. Parts like the body panels, which have an absolute position in the car lines e.g. the hood, and parts placed relative other parts e.g. wheels and engine components.

Absolute Position

The first group are placed fixed relative a general coordinate system of the car. This general car coordinate system is placed using the front axle as reference. One example is to place the x-axis along the length of the vehicle, the y-axis on top of the front axle and z axis vertical. In this case you will have right hand system with negative x-values in front of the axle and negative z-values underneath the front axle. Some companies have therefore moved the origin of the car a certain distance in front and underneath the car to avoid negative coordinates.

In common these car parts are positioned by superposition of the CATParts origins. Important are that the corresponding geometry has the correct position and orientation regarding the origin of the part. These parts will hang around in space at their position in the car lines. When being used as carry over parts their position has to be controlled.

Relative Position

The engine has its own reference coordinate system in a CATPart, in which a general skeleton is included. In this case constraints are used to position the engines sub-assemblies and components on the skeleton with assembly constraints. There are numerous levels of sub-assemblies in which sub-skeletons are found . It is here to recommend that the origin of the parts is placed on a clearly specified interface position. An origin which is used to assemble the parts.

These CATParts are examples of the second group. Their position is explicitly a result of the environmental components. Just as the wheels are being moved by a modification of the rear axle position, the position of the pistons are changed by a distance modification between the cylinders. Important is to have a placement of the origin, which adopt to the functional constraints.

Positions are important

2 mars 2017

Guidelines by sketcher

A very important skill, is how to use the Sketcher. By a great number of features you need to
define one or more sketches to define the outlook of these features. It is therefore of great importance that you are working with correct  guidelines and methods. Here is a list of the most important:

1) Fix position

The sketch itself shall be positioned regarding defined references with the option Positioned. Sliding shall not be used, since the sketch can unintentionally be moved from a modification without the user notice it.

2) Uncomplicated Geometry

Do not define a geometry with numerous ( more than ten ) elements (lines, arcs, curves...) but keep it simple. If your part is complicated divide the contour/section geometry into many sketches. Especially the first sketch should be simple and stable, due to the difficulties replacing it.

3) Fully Constrained

Use dimensions and geometrical constraints to unambiguous define the geometry. All the geometry elements shall be green. This is again to avoid any unattended modifications.

4) Without Fillets and Chamfers

Create the section/contour without any fillets/rounds or  chamfers. They would would make the sketch more complicated and therefore also less predictable  and  less stable.

5 ) Use Skeletons

If a complicated section/contour is to be defined it is certainly not a bad idea using a skeleton. The skeleton can be placed in its own sketch and be designed with untrimmed elements.

6) Exaggerate

Draw small elements bigger than they actually are. They will then be easier to dimension. Exaggerate also the angles to avoid making the program to assume the elements to be horizontal and vertical

If you want to practice and read more about correct sketches, you will find lessons and exercises in the branch sketcher