Verify your spacing in the CAM (Gerber) outputs. I trust that over what I see on the PADS screen, because...
PADS can be odd about the way it uses the line width when it draws. For example, the board outline is centered within the lines that are drawn, regardless of the line width. I use that to my advantage sometimes by setting my width to 40 mils when I draw the PCB outline, so it is very easy to see if anything violates the 20 mil item to PCB edge rule. When you draw a copper pour, the outer edge of the line defines the actual pour shape, so if you change the line width the outer edge doesn't move but the inner edge does, and your corner radii change.
I believe any hatch value less than your line width will result in a full pour.
Your line width does translate to Gerber aperture size. So if you want the fab to use their low cost process with 8/8 mil space/trace, don't define pours with a 1 mil line width.
I hope that helps.
I don't have my computer and using my memory (not a smartest thing to do)! Check your line width tof he copper shape was created versa hatch grid and try to adjusted. Inusualy I use small line width to make sure the pour will get into small craveses. Hatch grid I make a hair smaller then the line width. Remember for hatch to happen, system need feet two lines of copper shape into the space to fill it.
Other thing to do in Parameters is to check mark to remove violating thermals. Other parameter is the smoozing radius the shape will use.
That is all I got from my memory. Someone else can add more information if I missed something.
Actually I just use one hatch grid setting.
In the 'Drafting Properties' > 'Options' dialog set Hatch Grid to '0'. This is my default setting.
This will always make a continous flood regardless your copper outline is 0.2 or 0.5mm or whatever.
See attached picture.
I have used this setting for many years.
I think the answer that works about the best is a combination of everyone's input.
1. Set the Line Width to a little smaller than your minimum trace/space (for me, 0.15mm) ... (The 0.149mm setting removes the interface where 2 planes connect and form small acid trap "dimples".)
2. Set the default flood hatch settings grid and smooth radius to 0
3. Apply the setting, pour the copper, then VERIFY the output!
4. While you're at it ... Set the copper plane properties too.
This fills in without creating slivers that violate my minimum 0.15mm trace/space requirement.
Thanks for the summary!