Move selected parts of schematic to board

On 15.08.2016 18:42, Nick Sarzynski wrote:

I'm really not too sure if Eagle can do this but I have a schematic, a very large schematic with roughly 1800 components in it. I know that's a lot but its mainly resisters, caps and transistors with a hand full of IC's. What I want to know is if there is away to select a group of components on the schematic and bring just that selection to the board to roughly lay it out? I think P-cad can do this but I can't use that anymore. If I bring in the whole schematic over makes it impossible to place and route the components with the nasty ratsnest.

 

Does anybody know if this is possible? I'm very new to Eagle but not PCB design. Thanks!!

I had a quick go at an ULP that does this. If you group the stuff (at

schematic) run this ULP and it will be grouped in the board, ready to be

moved. You may play yourself adding this to a context menu.

Here is my result:

-

string g[];

int i=0;

project.schematic(S) S.parts(P) P.instances(I) if(ingroup(I))

{

     g[i++]=P.name;

     continue;

}

int x;

project.board(B)

{

     clrgroup(B);

     B.elements(E)

     {

          for(x=0;x<i;x++) if(E.name==g[x])

          {

               setgroup(E);

               continue;     

          }

     }

}

-

On 15.08.2016 18:42, Nick Sarzynski wrote:

I'm really not too sure if Eagle can do this but I have a schematic, a very large schematic with roughly 1800 components in it. I know that's a lot but its mainly resisters, caps and transistors with a hand full of IC's. What I want to know is if there is away to select a group of components on the schematic and bring just that selection to the board to roughly lay it out? I think P-cad can do this but I can't use that anymore. If I bring in the whole schematic over makes it impossible to place and route the components with the nasty ratsnest.

 

Does anybody know if this is possible? I'm very new to Eagle but not PCB design. Thanks!!

I had a quick go at an ULP that does this. If you group the stuff (at

schematic) run this ULP and it will be grouped in the board, ready to be

moved. You may play yourself adding this to a context menu.

Here is my result:

-

string g[];

int i=0;

project.schematic(S) S.parts(P) P.instances(I) if(ingroup(I))

{

     g[i++]=P.name;

     continue;

}

int x;

project.board(B)

{

     clrgroup(B);

     B.elements(E)

     {

          for(x=0;x<i;x++) if(E.name==g[x])

          {

               setgroup(E);

               continue;     

          }

     }

}

-

Nick Sarzynski wrote:

I'm really not too sure if Eagle can do this but I have a schematic, a

very large schematic with roughly 1800 components in it. I know that's

a lot but its mainly resisters, caps and transistors with a hand full

of IC's. What I want to know is if there is away to select a group of

components on the schematic and bring just that selection to the board

to roughly lay it out? I think P-cad can do this but I can't use that

anymore. If I bring in the whole schematic over makes it impossible to

place and route the components with the nasty ratsnest.

see

http://www.eaglecentral.ca/index.php/mv/msg/49208/154023/74df04597c8c5e4a78db11ddf52c8597/#msg_154023

for an ULP that will pick up parts grouped in the schematic in the

board editor.

--

Lorenz

Nick Sarzynski wrote:

I'm really not too sure if Eagle can do this but I have a schematic, a

very large schematic with roughly 1800 components in it. I know that's

a lot but its mainly resisters, caps and transistors with a hand full

of IC's. What I want to know is if there is away to select a group of

components on the schematic and bring just that selection to the board

to roughly lay it out? I think P-cad can do this but I can't use that

anymore. If I bring in the whole schematic over makes it impossible to

place and route the components with the nasty ratsnest.

see

http://www.eaglecentral.ca/index.php/mv/msg/49208/154023/74df04597c8c5e4a78db11ddf52c8597/#msg_154023

for an ULP that will pick up parts grouped in the schematic in the

board editor.

--

Lorenz

On 8/15/2016 12:42 PM, Nick Sarzynski wrote:

I'm really not too sure if Eagle can do this but I have a schematic, a very large schematic with roughly 1800 components in it. I know that's a lot but its mainly resisters, caps and transistors with a hand full of IC's. What I want to know is if there is away to select a group of components on the schematic and bring just that selection to the board to roughly lay it out? I think P-cad can do this but I can't use that anymore. If I bring in the whole schematic over makes it impossible to place and route the components with the nasty ratsnest.

 

Does anybody know if this is possible? I'm very new to Eagle but not PCB design. Thanks!!

 

--

To view any images and attachments in this post, visit:

https://www.element14.com/community/message/203677

 

Hi Nick,

I hope you're doing well. As has already been described when you go from

schematic to board all of the components will come over. One thing that

may help is to separate the schematic into various sheets.

Then you can use the group-aps_V4.ulp that's up on our website to

organize the parts into groups which you can then route individually.

Let me know if there's anything else I can do for you.

Best Regards,

Jorge Garcia

Hi Nick,

With the way EAGLE works ALL the components will appear in the board, there isn't a lot you can do about that I'm afraid.

However, there are a couple of things you can do:

1) Your biggest problem seems to be the ratsnest or air wires. You can turn off groups of air wires to make things easier to see. For example:

RATSNEST ! +5V0D 0VD AGND

would turn off all the air wires for the nets +5V0D 0VD and AGND.

You can even turn off all air wires with:

RATSNEST ! *

And then turn them on specifically for the nets in the group you wish to route so they are the only ones visible (may be a bit fiddly)

You can turn them all back on again with:

RATSNEST *

2) There are some ULP which will allow you to select groups of components in the schematic and then group move them in the layout so you can grab a bunch of related stuff in one hit and place it down away from all the rest of the unplaced stuff. I have a ULP called pickgrouped.ulp which I obtained from another member here when I was first starting out with EAGLE and it helped me out a lot on the first big design I had to do using it. You can find this ULP if you look at the answer marked as the correct answer from this thread: How can I select components booth in schematic and layout at the same time?

Best Regards,

Rachael

You did not specify what you want (criteria), but a ULP (like a program) can go through the components and affect some changes. Maybe one has been written if you look around. If not find one close and modify it.

Clem