Topics

Fat Library


John Johnson <johnatl@...>
 

Someone asked about the Fat Library mentioned in the docs, Art, I think?
A while back I found a way to do the same thing much more easily, using the DRC (Design Rules Check).
I'll look up the info this evening and post to the list.

Just didn't want you to think I had forgotten about you :-)

Regards,
JJ

---
Help everyone. If you can't do that, then at least be nice.


Art Eckstein <a_eckstein@...>
 

Thanks JJ, I figured you would when you got a chance!

Hope to see you sometime when you get down here! Give me a call.

Art

At 10:41 AM 12/14/2005, you wrote:
Someone asked about the Fat Library mentioned in the docs, Art, I think?
A while back I found a way to do the same thing much more easily, using
the DRC (Design Rules Check).
I'll look up the info this evening and post to the list.

Just didn't want you to think I had forgotten about you :-)

Regards,
JJ

---
Help everyone. If you can't do that, then at least be nice.


John Johnson <johnatl@...>
 

Art,

I uploaded pcb-gcode.dru into the Files section.
http://groups.yahoo.com/group/pcb-gcode/files/
Download and save into your Eagle/dru folder.
From the Board Editor, click the DRC button (In the tool bar on the left, bottom group of buttons.).
Click the Load... button.
Browse for the file pcb-gcode.dru.
Click the Check button.

The following errors and settings are available in DRC (Design Rule Check).

Width of tracks
If the tracks are wide enough in your opinion, in DRC, go to the Sizes tab and change the Minimum Width to something suitable for you.

Clearance
If the clearance between items (tracks, pads, etc.) is enough for your machine, go to DRC. On the Clearance tab, adjust the clearances accordingly.

Dimension
If you get a dimension error (track to close to a dimension line), you can adjust the accepted distance by going to DRC, then the Distance tab.

Pads
The size of the pads is calculated in the Restring tab of the DRC. The width of the pad is based on the diameter of the drill hole in the pad. In pcb-gcode.dru, you'll see the Top pads are set to min: 22 mil, 50%, max: 22 mil. Simply put, you're going to get a 22 mil pad. That is because both the Min and Max is set to 22 mils. If you change the Min to 10 mil (for instance), you will get a 64 mil pad. Here's how: the drill is 32 mil. The percentage for Top and Bottom is set for 50%. 50% of 32 mils is 16 mils. So, you have a 32 mil hole, with 16 mils on each side. 32 + 16 + 16 = 64 mils. (A mil is 0.001").

Pad Shapes
On the Shapes tab, you can control the shapes of the pads. In pcb-gcode.dru, Elongation% is set to 150%, 150%. The first 150% is the length of pads centered around the drill hole. If the pad is 64 mils wide (see above for setting the width), the length of the pad will be: 64 * 1.50 = 96 mils. The second number is for offset pads. The length is calculated the same, but the clearance calculated for one side of the pad (see above) is used on one end. Assuming the same 64 mils width and 32 mils drill, you would have 16 mils on three sides on the drill hole, the longest part of the pad would be 80 mils from the edge of the drill hole, for a total of 96 mils in length.
You can also change the default pad shapes using the Top, Bottom, and First drop down lists.

Supply
If you add a ground or supply plane to your board, the settings on the Supply tab of the DRC control the spacing and shape of the thermals, vias, and annuli. Setting Thermal Isolate higher makes thermals easier to solder, since there is more open space around them. Gap is calculated the same way that Pad size is (see above).

Masks
Sorry, I don't use them. Calculations appear to be the same as Pads (see above).

Misc
Checks for grid, angle, etc.

Regards,
JJ

On 15-Dec-2005, at 07:38, Art Eckstein wrote:

Thanks JJ, I figured you would when you got a chance!

Hope to see you sometime when you get down here! Give me a call.

Art

At 10:41 AM 12/14/2005, you wrote:
Someone asked about the Fat Library mentioned in the docs, Art, I think?
A while back I found a way to do the same thing much more easily, using
the DRC (Design Rules Check).
I'll look up the info this evening and post to the list.

Just didn't want you to think I had forgotten about you :-)

Regards,
JJ

---
Help everyone. If you can't do that, then at least be nice.






Yahoo! Groups Links







---
Help everyone. If you can't do that, then at least be nice.


Art Eckstein <a_eckstein@...>
 

JJ,
Thanks for the upload, I've got it and after I cet some coffee in me,
will give it a try :-D

Hopefully sometime this coming week, will be able to try my first
board. I have my plans all cadded up for making a stage to mount the
blank board. Just need to get into the shop and start fabrication.
But that is going to depend on weather as I have no heat in there and
it is not suited to heating either. Maybe it will warm up enough so I
can get up there today and at least get started.


Later,

Art

At 10:14 PM 12/16/2005, you wrote:
Art,

I uploaded pcb-gcode.dru into the Files section.
http://groups.yahoo.com/group/pcb-gcode/files/
Download and save into your Eagle/dru folder.
From the Board Editor, click the DRC button (In the tool bar on the
left, bottom group of buttons.).
Click the Load... button.
Browse for the file pcb-gcode.dru.
Click the Check button.

The following errors and settings are available in DRC (Design Rule
Check).

Width of tracks
If the tracks are wide enough in your opinion, in DRC, go to the Sizes
tab and change the Minimum Width to something suitable for you.

Clearance
If the clearance between items (tracks, pads, etc.) is enough for your
machine, go to DRC. On the Clearance tab, adjust the clearances
accordingly.

Dimension
If you get a dimension error (track to close to a dimension line), you
can adjust the accepted distance by going to DRC, then the Distance
tab.

Pads
The size of the pads is calculated in the Restring tab of the DRC. The
width of the pad is based on the diameter of the drill hole in the pad.
In pcb-gcode.dru, you'll see the Top pads are set to min: 22 mil, 50%,
max: 22 mil. Simply put, you're going to get a 22 mil pad. That is
because both the Min and Max is set to 22 mils. If you change the Min
to 10 mil (for instance), you will get a 64 mil pad. Here's how: the
drill is 32 mil. The percentage for Top and Bottom is set for 50%. 50%
of 32 mils is 16 mils. So, you have a 32 mil hole, with 16 mils on each
side. 32 + 16 + 16 = 64 mils. (A mil is 0.001").

Pad Shapes
On the Shapes tab, you can control the shapes of the pads. In
pcb-gcode.dru, Elongation% is set to 150%, 150%. The first 150% is the
length of pads centered around the drill hole. If the pad is 64 mils
wide (see above for setting the width), the length of the pad will be:
64 * 1.50 = 96 mils. The second number is for offset pads. The length
is calculated the same, but the clearance calculated for one side of
the pad (see above) is used on one end. Assuming the same 64 mils width
and 32 mils drill, you would have 16 mils on three sides on the drill
hole, the longest part of the pad would be 80 mils from the edge of the
drill hole, for a total of 96 mils in length.
You can also change the default pad shapes using the Top, Bottom, and
First drop down lists.

Supply
If you add a ground or supply plane to your board, the settings on the
Supply tab of the DRC control the spacing and shape of the thermals,
vias, and annuli. Setting Thermal Isolate higher makes thermals easier
to solder, since there is more open space around them. Gap is
calculated the same way that Pad size is (see above).

Masks
Sorry, I don't use them. Calculations appear to be the same as Pads
(see above).

Misc
Checks for grid, angle, etc.

Regards,
JJ

On 15-Dec-2005, at 07:38, Art Eckstein wrote:

Thanks JJ, I figured you would when you got a chance!

Hope to see you sometime when you get down here! Give me a call.

Art

At 10:41 AM 12/14/2005, you wrote:
Someone asked about the Fat Library mentioned in the docs, Art, I
think?
A while back I found a way to do the same thing much more easily,
using
the DRC (Design Rules Check).
I'll look up the info this evening and post to the list.

Just didn't want you to think I had forgotten about you :-)

Regards,
JJ

---
Help everyone. If you can't do that, then at least be nice.