Trace end square

Hi Nicolas

So what you could do there is change the segment width of the trace before you connect to the pin. But for SMD packages there is a better way and that is to use Shapes. Here is a pic to illustrate.

Looks pretty good eh. Anyway try using shapes for certain things beyond your average ground plane. With shapes it is possible to get really great results coming off pins etc, far more than traditional traces.
The trick is to mix and match the best options to do what you need.

Maybe this will help you out

All the best

Oh excellent ! I agree I’ll get better looking results with. I tried as you can see from the top picture. I made a square shape to join all four pins of the two p-fet at the bottom on net N01483 and at the top on N02134. I wasn’t sure of the options to choose from. There was dynamic and static copper. Which one I should choose ? Will the trace connect to the shape instead of the pad ? I tried but it did not seem to let me connect the net to the shape but still wanted to connect to the pad. Maybe I am missing something here. Can you light up my lantern on that please  

thanks, 

So when it comes to shapes there are both dynamic & static types. Dynamic would be your traditional copper pour that can automatically void around traces. Static are just Static. In the prior picture the shapes I used are static types as they offer tight control.

When you create a shape that you wish to connect to a pin you have to think in terms of Nets. So assume your pin has a net name of 12V and you want a shape to connect to that pin you would need to assign a net to the shape. To do this you use the options panel. There is a box there called "Assign a net name" choose the net name you want to use. Then draw your shape. You have to click on the shape type first then go to the options panel to choose the net.

In the options panel you will also see the type of shape your wanting to use, Static or Dynamic. Choose the right one.

What I do is typically draw a shape rectangle then come back later and carve it up or resize it. To carve things up try the shape edit boundary.You could also choose Shape Add, the icon that looks like an L backwards. This option will allow you to draw more complex shapes.

Here is another pic.

.

You can use traces to connect to the shape, Provided the trace has the same net name otherwise your going to end up with drc errors. In the picture you can see the pads highlighted in blue and I am routing a trace from the shape at C12 to the pin on the smd cap on the left. When the connect is made the rat line will disappear.

To start out I think static shapes may give you the best results. When you add the shape that connects to a pin/pad it is usually good to have the shape hitting the center of the pin as you draw the shape in.

In the Cadence Allegro/Orcad PCB tools shapes are a real gem. With these tools you can create about any type of etch you want. It is worth the time to dig in and learn all about shapes. I live in the RF world so needless to say I am highly biased to shapes

All the best.

This awesome ! Exactly what I wanted. I'll give it a try and experiment all this. It is interesting to learn that create a manual net even if I don't pick it up from the rats on the pad will complete it. 

Thanks once again for taking the time to answer my questions. This is appreciated. 

Regards,