CATIA V5 - Sketch analysis

After you finish the drawing (sketch) it is good to check the suitability of the sketch for further work. With this in mind, it is necessary to check that all lines and radii are in line with our wishes. The biggest problem is the "openness" of the model or the draft, since this may be the cause of the mismatch in further work and may disable the development of the model.

In order to avoid such problems, a CATIA software is a very useful tool that allows you to check the convenience of the sketch for further work with a single click. With this tool, we can also check if there is a sketch, for example, double lines, open or unfinished profiles or overlaps.

When we finish the sketch, we run Sketch AnalysisSketch Analysis_ON _tools_catia_v5

The tool is located inside the SKETCHER module and is intended to detect errors on the sketch.

You can easily access the tool using the TOOLS -> SKETCH ANALYSIS drop-down menu, but also through the toolbar.

Then we open a working window with the results of the analysis, and at the same time sketch shows possible errors or anomalies. In the example shown in Figure 2, you can see that the model is open - the green colour indicates the distance between the two open points, marked with a blue color.


example_results_sketch_analysis_catia_v5

Figure 1.  Example of the Sketch Analysis result


Inside the window with the results of the analysis, the first GEOMETRY card (1) shows the description of the sketch, where we can see the details of the analysis and error:

  • In the Geometry column (1) there is a description of the profile description that we have drawn
  • The results shown in the Status column indicate whether the profile is open or closed. An open profile means that the lines are not completed or connected.
  • A closed profile means that the sketch is closed or closed. The Comment column contains a precise profile description.
  • If the profile is open, it tells us the distance of the end point of the profile. Distance is given in millimeters and represents the distance between the blue spots in the figure.

Within the analysis itself, we can find additional shortcuts, called Corrective Actions, with which they can fix sketches, create helplines, close the profile automatically, delete angles, etc.

The third Diagnostic card (2) shows whether the sketch is defined, or whether the individual points or lines are exactly defined in terms of the reference / zero position of the coordinate system (shown in Figure 2 in yellow - 4).


CATIA_v5_diagnostic_card

Figure 2. The "Diagnostic" tab

  • Interpretation of terms appearing in the Diagnostic tab:

    ISO-Constrained: defined in relation to the starting position
    • Under-Constrained: not defined in relation to the starting position
     


You can easily find undefined points and lines by right-clicking on a specific point or line, and in the drop-down menu by choosing Reframe on (5), shown in Figure 3.


catia_v5_reframe_diagnostic_cardFigure 3. „Reframe on“ in tab „Diagnostic“

This operation will show us exactly the selected line or point, in the middle of the screen, so that we can find it easier.


catia_v5_display_the_line_selected_using_the_reframe_on_function

Figure 4: Display the line selected using the "Reframe on" function


If Center Graph (6) is selected in the drop-down menu, the selected line will be marked with orange in the tree of the model (Figure 5).


catia_v5_model_tree_center_graph

Figure 5. Model tree when using the "Center Graph" function