Change Footprint AFTER routing Protel 99SE???

[mike]

Protel 99SE.
I made a metric footprint for a TQFP64 package.
board looks good in the gerber, but when I try to plot it,
I get traces overlapping.

I think the problem is because I have a metric footprint,
an unfortunate combination of imperial routing grid and snap grid,
and a plotter with 5mil resolution. The roundoff error in
all the conversion processes to get to the plotter is killing me.
I think I can fix it by replacing the metric footprint with an
imperial one. The actual dimensional changes are very tiny.

I can't figure out how to swap the new footprint into the
board layout without unrouting everything.

I thought "refresh parts in cache" would do it, but doesn't seem to.

Ideas? I really, really don't want to do the layout again.

Thanks, mike
--
Return address is VALID.
500MHz Tek DSOscilloscope TDS540 $2200
http://nm7u.tripod.com/homepage/te.html
Wanted, 12.1" LCD for Gateway Solo 5300. Samsung LT121SU-121
Bunch of stuff For Sale and Wanted at the link below.
http://www.geocities.com/SiliconValley/Monitor/4710/

 

[mike]

Brad Velander wrote:

Mike,

It should work exactly as Spehro states. Just make sure that
you have used the same reference point when making both
footprints in the library. One alternative method would be to
edit the existing footprint in the library, then just click the
"Update PCB" button while you have the PCB file open in Protel.
I would make a second footprint though and keep the original as
well.
As far as your overall problem goes, it would seem to more of
a printer issue. I don't think changing the footprint to an
imperial version is going to do anything for you.
Also, when you place the new part no traces are going to
automagically snap into place for you. You will have to cleanup
the last segment or two of the routes manually where they
misalign.

Thanks for the input, I'll try it.

I'm not exactly sure what you mean by reference point. It's currently
pin 1. I am definitely going to have to move the origin and introduce
a .0025 mil error in one dimension to get all the pads exactly on the 5
mil grid in both axes.

So far, I've been unable to update the footprint. Seems that refreshing
the screen doesn't show the changes until I change to the next part in
the library then back to the one I'm editing. Had pads six deep from
previous attempts to move stuff. Now that I know about the quirk, I
should be able to make it happen.

I think it's definitely a printer...or in this case a plotter problem.
Plotter has 5mil resolution. Placement grid was 1mil, routing grid was
16 mil for some unknown reason. The plotter is rounding the coordinate
to the nearest 5mil position. When you only have 5 mils between traces,
this is a disaster. I'm hoping when I get everything registered on a
5 mil grid, I'll be able to plot it...I hope.

I'm trying to plot this on copper to make the board. Registration is
critical. Sure wish I'd figgered this out before I spent all the time
on the layout ;-)
mike

--
Return address is VALID.
500MHz Tek DSOscilloscope TDS540 $2200
http://nm7u.tripod.com/homepage/te.html
Wanted, 12.1" LCD for Gateway Solo 5300. Samsung LT121SU-121
Bunch of stuff For Sale and Wanted at the link below.
http://www.geocities.com/SiliconValley/Monitor/4710/

 

[Brad Velander]

Mike,
The reference location for library parts in Protel is always
0,0 when you made the part. If the part is made offset from 0,0
you will notice that when you place the part you are moving it
around by some point that was where 0,0 was relative to the
footprint you designed in the library. Same for schematic symbols
except that commonly you put the 0,0 reference just at the
connection point of any pin. The issue with updating the part
footprint is that if the references weren't the same for both
versions of the footprint, the new footprint will come into your
design at a location offset from the original and you will have
to move it manually back into the desired location. If the offset
is on some very small grid (multiples of 0.01 mils, 0.00001
inches), precise relocation of the new footprint could be nearly
impossible but definitely frustrating.

Typically I design all SMT parts with 0,0 at the centroid
pick location. Others design them such that pin one is the
reference location (0,0). There is one caveat to using the pin
one reference. Protel generates Pick n Place files with 3
coordinates, the reference location, the calculated center of all
pads and the pin one location. With asymmetrical parts (DPAKS,
TO263, TO252, etc.) Protel cannot calculate the correct center of
the device based upon the pads because the pads are not centered
within the part outline.

Protel does have an annoying habit of not refreshing the
screen as much as they should. This is undoubtedly why you were
seeing multiple pad locations onscreen. Just get used to using V,
R (View Refresh) often while performing some operations. It is
just second nature to me after years. If I pause slightly in my
work, my immediate response is to hit V, R.
Hold it, I just reread your response. Sounds like your
refresh issue is something else. Could it be video card related?
Protel hates the older (3 - 5 years) ATI cards. I thought it was
the simple refresh issue when I first read it.

--
Sincerely,
Brad Velander

"mike" <spamme0@netscape.net> wrote in message
news:4191EC01.10107@netscape.net...

Brad Velander wrote:

Thanks for the input, I'll try it.

I'm not exactly sure what you mean by reference point. It's
currently
pin 1. I am definitely going to have to move the origin and
introduce
a .0025 mil error in one dimension to get all the pads exactly
on the 5
mil grid in both axes.

So far, I've been unable to update the footprint. Seems that
refreshing
the screen doesn't show the changes until I change to the next
part in
the library then back to the one I'm editing. Had pads six
deep from
previous attempts to move stuff. Now that I know about the
quirk, I
should be able to make it happen.

I think it's definitely a printer...or in this case a plotter
problem.
Plotter has 5mil resolution. Placement grid was 1mil, routing
grid was
16 mil for some unknown reason. The plotter is rounding the
coordinate
to the nearest 5mil position. When you only have 5 mils
between traces,
this is a disaster. I'm hoping when I get everything
registered on a
5 mil grid, I'll be able to plot it...I hope.

I'm trying to plot this on copper to make the board.
Registration is
critical. Sure wish I'd figgered this out before I spent all
the time
on the layout ;-)
mike

--

 

[mike]

Brad Velander wrote:

Mike,
The reference location for library parts in Protel is always
0,0 when you made the part. If the part is made offset from 0,0
you will notice that when you place the part you are moving it
around by some point that was where 0,0 was relative to the
footprint you designed in the library. Same for schematic symbols
except that commonly you put the 0,0 reference just at the
connection point of any pin. The issue with updating the part
footprint is that if the references weren't the same for both
versions of the footprint, the new footprint will come into your
design at a location offset from the original and you will have
to move it manually back into the desired location. If the offset
is on some very small grid (multiples of 0.01 mils, 0.00001
inches), precise relocation of the new footprint could be nearly
impossible but definitely frustrating.

Not a problem. I really want it in a different place so all the
connections line up exactly on a 5mil grid. As long as it doesn't
disconnect itself or unroute, I'm ok. I'm jumping thru hoops here to
work around using a plotter that's BARELY up to the task.

Typically I design all SMT parts with 0,0 at the centroid
pick location. Others design them such that pin one is the
reference location (0,0). There is one caveat to using the pin
one reference. Protel generates Pick n Place files with 3
coordinates, the reference location, the calculated center of all
pads and the pin one location. With asymmetrical parts (DPAKS,
TO263, TO252, etc.) Protel cannot calculate the correct center of
the device based upon the pads because the pads are not centered
within the part outline.

Protel does have an annoying habit of not refreshing the
screen as much as they should. This is undoubtedly why you were
seeing multiple pad locations onscreen. Just get used to using V,
R (View Refresh) often while performing some operations. It is
just second nature to me after years. If I pause slightly in my
work, my immediate response is to hit V, R.

Yep, V, R doesn't do it. had to change to the next part in the library
and back to get all the elements to show. Video card is a Trident
9750... definitely old.

I don't use Protel very much and have to relearn everything every time
I use it.

You sound like you know the tool well...
Is there a tutorial on making the autorouter do your bidding?
I have one TQFP64 microcontroller that gets routed to a 40-pin dip
header. Every time I run the autorouter, I get a different route.
If I move the header ever so slightly, I get a WILDLY different route.
Often, it threads a track back and forth between dip pins when
there's a direct routing channel available. I try keepout traces and
layers to block access from the not preferred direction. Sometimes this
works, but others, it just causes things to get worse.

I'm routing a single layer board.

Oh, another annoying thing it does is claim to be 100% routed when it
still has a dozen nets shorted together.

mike

Hold it, I just reread your response. Sounds like your
refresh issue is something else. Could it be video card related?
Protel hates the older (3 - 5 years) ATI cards. I thought it was
the simple refresh issue when I first read it.

--
Return address is VALID.
500MHz Tek DSOscilloscope TDS540 $2200
http://nm7u.tripod.com/homepage/te.html
Wanted, 12.1" LCD for Gateway Solo 5300. Samsung LT121SU-121
Bunch of stuff For Sale and Wanted at the link below.
http://www.geocities.com/SiliconValley/Monitor/4710/

 

[Clarence]

"mike" <spamme0@netscape.net> wrote in message
news:419342C4.2020804@netscape.net...

Brad Velander wrote:
Mike,
The reference location for library parts in Protel is always
0,0 when you made the part. If the part is made offset from 0,0
you will notice that when you place the part you are moving it
around by some point that was where 0,0 was relative to the
footprint you designed in the library. Same for schematic symbols
except that commonly you put the 0,0 reference just at the
connection point of any pin. The issue with updating the part
footprint is that if the references weren't the same for both
versions of the footprint, the new footprint will come into your
design at a location offset from the original and you will have
to move it manually back into the desired location. If the offset
is on some very small grid (multiples of 0.01 mils, 0.00001
inches), precise relocation of the new footprint could be nearly
impossible but definitely frustrating.

Not a problem. I really want it in a different place so all the
connections line up exactly on a 5mil grid. As long as it doesn't
disconnect itself or unroute, I'm ok. I'm jumping thru hoops here to
work around using a plotter that's BARELY up to the task.


Typically I design all SMT parts with 0,0 at the centroid
pick location. Others design them such that pin one is the
reference location (0,0). There is one caveat to using the pin
one reference. Protel generates Pick n Place files with 3
coordinates, the reference location, the calculated center of all
pads and the pin one location. With asymmetrical parts (DPAKS,
TO263, TO252, etc.) Protel cannot calculate the correct center of
the device based upon the pads because the pads are not centered
within the part outline.

Protel does have an annoying habit of not refreshing the
screen as much as they should. This is undoubtedly why you were
seeing multiple pad locations onscreen. Just get used to using V,
R (View Refresh) often while performing some operations. It is
just second nature to me after years. If I pause slightly in my
work, my immediate response is to hit V, R.

Yep, V, R doesn't do it. had to change to the next part in the library
and back to get all the elements to show. Video card is a Trident
9750... definitely old.

I don't use Protel very much and have to relearn everything every time
I use it.

You sound like you know the tool well...
Is there a tutorial on making the autorouter do your bidding?
I have one TQFP64 microcontroller that gets routed to a 40-pin dip
header. Every time I run the autorouter, I get a different route.
If I move the header ever so slightly, I get a WILDLY different route.
Often, it threads a track back and forth between dip pins when
there's a direct routing channel available. I try keepout traces and
layers to block access from the not preferred direction. Sometimes this
works, but others, it just causes things to get worse.

I'm routing a single layer board.

Oh, another annoying thing it does is claim to be 100% routed when it
still has a dozen nets shorted together.

mike

You need to adjust your layout rules. If there is insufficient space under the
rules given it will try to complete and allow you to "Clean up" the errors.

 

[Brad Velander]

Mike,
I checked my archives of Protel documents and I don't have
anything on the autorouter. Nothing beyond the couple of pages in
their manual or general P99SE tutorials. Typical, it is supposed
to work magically, if you needed a manual then it obviously
doesn't work as well as it should. Rrrrriiiggghhhtt!

Try the Protel EDA list server, I know there are newbies and
hobbyists on there periodically. The guys on the list are a very
fine group of people and they will do everything in their power
to help you as long as you aren't using them just as an online
version of the manuals, so that you don't have to read them
yourself.

I have never made an autorouter do anything near right, so I
can't comment on the Orcad stuff either. I have always pined for
a company that would lay out the bucks for an upper level Cooper
Chyan autorouter and the course to teach me how to really use it
properly. At least with their routers I know the upper-end
versions will handle most of the rules required for my typical
designs.

--
Sincerely,
Brad Velander

"mike" <spamme0@netscape.net> wrote in message
news:4193ECBA.8080805@netscape.net...

Not that simple. I'm plotting resist on copper and etching
the board
directly from the plot. I know it's beyond the capability of
the
process, but the chip don't come in a bigger package and I
don't have
the option to change the chip. It's becoming a moot point,
because
I can't find a pen with a fine enough tip with ink that
'resists' the
etchant.

We're attempting to build the flash update for a picstart+
programmer.
Can buy a pair of upgrade boards for $60, so this project is
more of
a "me against the tool" challenge than an economic benefit.
I'm
retired, so if I didn't waste my time on this, I'd have to find
something else to waste it on...

As it's a questionable hobby project, I try to limit my
questions on the
web. You professionals have enough of your own stuff to worry
about
without me bothering you.

I've been using a DOS version of PADS. Switched to Protel
because it
runs under windows and I can get more stuff on the higher res
screen
and was free. Even when I help it, it wants to fly off in
another
direction and do other stupid things. I expect convergence to
a good
route, especially when there are obvious better
paths...straiaght shot,
nothing in the way...short distance...
I don't remember having these kinds of routing issues with
PADS, but
it's been a long time. I may have to try switching back.
I'm stuck with tools that can be had for free.
That limits my choices ;-)
I have Orcad 9 something laying around. Is that autorouter any
better?
mike

 

[Spehro Pefhany]

On Tue, 09 Nov 2004 18:37:30 -0800, the renowned mike
<spamme0@netscape.net> wrote:

Protel 99SE.
I made a metric footprint for a TQFP64 package.
board looks good in the gerber, but when I try to plot it,
I get traces overlapping.

I think the problem is because I have a metric footprint,
an unfortunate combination of imperial routing grid and snap grid,
and a plotter with 5mil resolution. The roundoff error in
all the conversion processes to get to the plotter is killing me.
I think I can fix it by replacing the metric footprint with an
imperial one. The actual dimensional changes are very tiny.

I can't figure out how to swap the new footprint into the
board layout without unrouting everything.

I thought "refresh parts in cache" would do it, but doesn't seem to.

Ideas? I really, really don't want to do the layout again.

Thanks, mike

I think if you just double click on the part and change the footprint
to the new name (in Properties) it will work.


Best regards,
Spehro Pefhany
--
"it's the network..." "The Journey is the reward"
speff@interlog.com Info for manufacturers: http://www.trexon.com
Embedded software/hardware/analog Info for designers: http://www.speff.com

 

[Brad Velander]

Mike,

It should work exactly as Spehro states. Just make sure that
you have used the same reference point when making both
footprints in the library. One alternative method would be to
edit the existing footprint in the library, then just click the
"Update PCB" button while you have the PCB file open in Protel.
I would make a second footprint though and keep the original as
well.
As far as your overall problem goes, it would seem to more of
a printer issue. I don't think changing the footprint to an
imperial version is going to do anything for you.
Also, when you place the new part no traces are going to
automagically snap into place for you. You will have to cleanup
the last segment or two of the routes manually where they
misalign.

--
Sincerely,
Brad Velander

"Spehro Pefhany" <speffSNIP@interlogDOTyou.knowwhat> wrote in
message news:5c13p0tafgg895g49qvl01i62i190n110f@4ax.com...

On Tue, 09 Nov 2004 18:37:30 -0800, the renowned mike

I think if you just double click on the part and change the
footprint
to the new name (in Properties) it will work.


Best regards,
Spehro Pefhany
--
"it's the network..." "The Journey is
the reward"
speff@interlog.com Info for manufacturers:
http://www.trexon.com
Embedded software/hardware/analog Info for designers:
http://www.speff.com

 

[Brad Velander]

Hi Mike,
Yes I know the tool fairly well, been using it day in and out
for about 5 years now. It is definitely not without it's quirks
but then I have never found a CAD tool that wasn't. A lot of the
disparaging comments about one package or the other only come
from people who haven't used most of them that far past an
initial canned tutorial stage. Over my career I have used a lot
of the medium priced tools ($5,000 - $20,000) for some period of
time.

Since your main problem would seem to be your plotter, do you
not have a friend or acquaintance with either a better plotter or
a laser that could do the actual prints for you? Set your machine
with the appropriate driver and print to a file. Take (or email)
the file to their place and plot or print it out? Possibly even a
plotting service, fab house or design bureau may do this for a
minimal charge.

Yes the Protel autotooter! It is to a large degree just a
tool for the salesmen to use when tooting their package to
unknowledgeable department managers. I know some people that seem
to be able to use it with reasonable results but most just don't
even try to use it after playing with it for a few days. That is
the same scenario with me, I played with it for a number of days
then gave up when anything I tried couldn't stop the nonsense
that it would route. I will take a look at work and see if I have
any tutorials on the autorouter. Most of the P99SE documentation
on the Protel website has slowly vanished over the past few years
but I have a bunch archived at work.

One resource that you should know about is the Protel EDA
listserver. It is an independent listserver with professional
Protel users around the world. Most are in North America or
Australia but a number are from Europe and a few in Asia as well.
You can usually get good advice and assistance from other users
within a couple of hours no matter what time of the day or night.
Check it out at:

http://www.techservinc.com/protelusers/index.html

There are a number of users on the listserver that do claim
to be able to get the autorouter to work reasonably well for
digital designs. One other reason that I don't use it is that my
PCB designs are typical mixed analog/digital, RF or even high end
microwave, so the Protel autorouter is just not up to that task
because of it's limited rules capability.


--
Sincerely,
Brad Velander


"mike" <spamme0@netscape.net> wrote in message
news:419342C4.2020804@netscape.net...

Not a problem. I really want it in a different place so all
the
connections line up exactly on a 5mil grid. As long as it
doesn't
disconnect itself or unroute, I'm ok. I'm jumping thru hoops
here to
work around using a plotter that's BARELY up to the task.


Yep, V, R doesn't do it. had to change to the next part in the
library
and back to get all the elements to show. Video card is a
Trident
9750... definitely old.

I don't use Protel very much and have to relearn everything
every time
I use it.

You sound like you know the tool well...
Is there a tutorial on making the autorouter do your bidding?
I have one TQFP64 microcontroller that gets routed to a 40-pin
dip
header. Every time I run the autorouter, I get a different
route.
If I move the header ever so slightly, I get a WILDLY different
route.
Often, it threads a track back and forth between dip pins when
there's a direct routing channel available. I try keepout
traces and
layers to block access from the not preferred direction.
Sometimes this
works, but others, it just causes things to get worse.

I'm routing a single layer board.

Oh, another annoying thing it does is claim to be 100% routed
when it
still has a dozen nets shorted together.

mike

 

[mike]

Brad Velander wrote:

Hi Mike,
Yes I know the tool fairly well, been using it day in and out
for about 5 years now. It is definitely not without it's quirks
but then I have never found a CAD tool that wasn't. A lot of the
disparaging comments about one package or the other only come
from people who haven't used most of them that far past an
initial canned tutorial stage. Over my career I have used a lot
of the medium priced tools ($5,000 - $20,000) for some period of
time.

Since your main problem would seem to be your plotter, do you
not have a friend or acquaintance with either a better plotter or
a laser that could do the actual prints for you? Set your machine
with the appropriate driver and print to a file. Take (or email)
the file to their place and plot or print it out? Possibly even a
plotting service, fab house or design bureau may do this for a
minimal charge.

Not that simple. I'm plotting resist on copper and etching the board
directly from the plot. I know it's beyond the capability of the
process, but the chip don't come in a bigger package and I don't have
the option to change the chip. It's becoming a moot point, because
I can't find a pen with a fine enough tip with ink that 'resists' the
etchant.

We're attempting to build the flash update for a picstart+ programmer.
Can buy a pair of upgrade boards for $60, so this project is more of
a "me against the tool" challenge than an economic benefit. I'm
retired, so if I didn't waste my time on this, I'd have to find
something else to waste it on...

As it's a questionable hobby project, I try to limit my questions on the
web. You professionals have enough of your own stuff to worry about
without me bothering you.

I've been using a DOS version of PADS. Switched to Protel because it
runs under windows and I can get more stuff on the higher res screen
and was free. Even when I help it, it wants to fly off in another
direction and do other stupid things. I expect convergence to a good
route, especially when there are obvious better paths...straiaght shot,
nothing in the way...short distance...
I don't remember having these kinds of routing issues with PADS, but
it's been a long time. I may have to try switching back.
I'm stuck with tools that can be had for free.
That limits my choices ;-)
I have Orcad 9 something laying around. Is that autorouter any better?
mike

Yes the Protel autotooter! It is to a large degree just a
tool for the salesmen to use when tooting their package to
unknowledgeable department managers. I know some people that seem
to be able to use it with reasonable results but most just don't
even try to use it after playing with it for a few days. That is
the same scenario with me, I played with it for a number of days
then gave up when anything I tried couldn't stop the nonsense
that it would route. I will take a look at work and see if I have
any tutorials on the autorouter. Most of the P99SE documentation
on the Protel website has slowly vanished over the past few years
but I have a bunch archived at work.

One resource that you should know about is the Protel EDA
listserver. It is an independent listserver with professional
Protel users around the world. Most are in North America or
Australia but a number are from Europe and a few in Asia as well.
You can usually get good advice and assistance from other users
within a couple of hours no matter what time of the day or night.
Check it out at:

http://www.techservinc.com/protelusers/index.html

There are a number of users on the listserver that do claim
to be able to get the autorouter to work reasonably well for
digital designs. One other reason that I don't use it is that my
PCB designs are typical mixed analog/digital, RF or even high end
microwave, so the Protel autorouter is just not up to that task
because of it's limited rules capability.

--
Return address is VALID.
500MHz Tek DSOscilloscope TDS540 $2200
http://nm7u.tripod.com/homepage/te.html
Wanted, 12.1" LCD for Gateway Solo 5300. Samsung LT121SU-121
Bunch of stuff For Sale and Wanted at the link below.
http://www.geocities.com/SiliconValley/Monitor/4710/