Hi, I'm a newbie.I have some problems with Orcad PCB Designed and thermal relief.I have edited a pad and defined this pad for all the layers:regular pad: circle 60thermal relief: circle 80antipad: circle 80When I create a dynamic shape to create a copper pour region the ray of thermal relief area is always of 5 mills.The part of copper pour between the spokes is only 5mills instead of 10mills [10=(80-60)/2].I have done a lot of attempts, changing pad parameters in the pad designer, but it doesn't workn. The size of the void spaces between the spokes of the thermal relief generated on the positive planes or dynamic shape is always the same.Thanks a lot.Carlo
The thermal relief line width is taken from 1 of the following
1. MIN_LINE_WIDTH property if one is set on the net. e.g. MIN_LINE_WIDTH = 10 MIL.2. The Physical constraint for MIN LINE WIDTH for that net and layer assignment. Look in Constarint Manager under Physical Constraint >All Layers.3. The shape parameter, either an instance based entry or global. Select Shape>Global Dynamic params...Selct the 'Thermal relief connects' tab. You can enter a fixed thermal width or an oversize. If you enter an oversize thermal with it will be added to the min line width specifed by the Physical constraint (#2 above) that that net class uses for line width.If you have a MIN_LINE_WIDTH property it will take precedence over the constraint and shape parameters.The void is derived from the spacing constraint Shape to pin (or via). You more than likely have a 5 MIL spacing constraint for the shape to element spacing set.The thermal and antipad definitions are used when constructing negative layers.
Thanks for your answare.
The problem is about the width of the void space between the spokes.I have set all spacing constraint at 12.00mills for my test, shape to pin and shape to vias too. I have update the dynamic shape but the size is always 5 mills.
I have found these on my book "Complete PCB Design Using OrCAD® Capture and PCB Editor":
Thermal relief connections between plated through holes and copper areas onpositive planes are automatically generated by PCB Editor so flash symbolsneed not be defined for positive layers. The inner diameter (ID) of the thermalrelief is defined by the pad diameter while the outer diameter (OD) is definedby the diameter of the (thermal relief) circle in the padstack definition set inthe Padstack Designer.
If I set a clearance oversize in Shape->Global Dynamic shape Parameters->Clearances Tab, for thru pin at 7mills the width of void space become 12mills(5+7) but the oversize is applied to the other type of pin, without thermal relief.
What is the way to set the size of thermal relief void space between the spokes, without changing the clearence between dynamic shape (copper pour) and the pin connected to the signal nets?
The spacing between the shape and pin is determined by the value for the 'Thru Pin to Shape Same Net Spacing' in Constraint Manager under Same Net Spacing >All Layers >Shape to <element> in this case the element is Pin.
Thank you very much