Displaying the borders of part section in the Visualization

You could first show the deformed plot and color code it by material (or section). Then create an overlay plot (View-Overlay plot) with this as your first layer. Now change the plot to a contour of stress, or whatever field you want. Go back to the overlay dialog and "create" another layer. Check the box to copy the view orientation from the first layer. Now click the "plot overlay" button. With the second (stress) plot as the one marked "current", go back to the common options (Options-Common...) and on the "other" tab choose the translucency setting. Play with the setting until you can see the underlying color of the color-coded layer.

OR
If you go to the Results Tree, expand the Output Databases branch, and expand the Materials branch. If you select a particular material it will highlight the appropriate elements.

OR
Create two viewports, tile the viewports, then link them so view manipulations apply simultaneously to both, but uncheck the option to link "plot states". In one viewport display shaded deformed mesh with color coding by material. In the other viewport display contours of stress. Now you can rotate the models together...

I'm sure there are other ways.

Hello brep
for the ifrst one it is really tedious to work with overlay and control the view through it. So I could not do it: sad
for the second : the problem is that all material elements appear when tou highlight them, which you can see but you cannot present it is very inappropriate to display in a presentation
for the third one
I created two viewports, tile the viewports, then link them I unchecked the option to link "plot states". In one viewport I displaied shaded deformed mesh with color coding by material. In the other viewport display contours of stress. But now how can link them they are not transperent from their viewports.
It is very important and basic for analyzing the results but really puzzling.
How can I show the borders of the materials of a part in the visualization

If you are worrying about result averaging (a post processing necessity) going across material boundaries, then there are a lot of controls for specifying the averaging boundaries. (BTW: By default Abaqus will *NOT* average across different sections)

Now i am not worried about that.
But if one looks at these countours, how can one know which contour line result for what material.The interpretation of results in a finite element model is made with reference to the materials composing the model

You can always select the elements associated with that material in the display manager and just plot contours for that particular material.

corus

Overlay plots are still your answer. Create one layer for your whole model with shaded stress contours. Create subsequent layers for each region of the model with a particular material (section) assignment. Hint: Use display groups to do this – it’s very easily done. Now plot all the layers. Go and edit “Common Plot options” for the layer of material 1 so that it is shaded with “free edges” shown. Then edit the edge thickness to be something more like the maximum. Finally make this plot 100% translucent. Repeat these options for the other layers of your materials. This worked for me, and took about 1 minute to set up for 4 material regions…

Berg ...Thank you. I made it with the help of your instructions
Corus.. I also appreciate your support