initial automatic component placement grid is wrong/how to change it

On 08/30/2014 03:54 PM, peter wrote:

I'm using Eagle Pro 6.6.

 

I noticed a behaviour that has me very frustrated and I can't find a way

to fix it.

 

If I create a Schematic with say 64 LED's (SMD devices to created with a

grid on 0.1mm in the library)

 

And wire them up appropriately in the schematic.

 

then switch to the PCB view, the 64 LED's are automatically placed on

the board outside of the default PCB area, but they are placed in a n

array  pattern that i have no control over, and that seems to be

slightly off when I then set the PB grid to 0.1mm for placement...

 

from row to row of LED's they are slightly misaligned when i pick them

up to place them they don't line up correctly with LED's that were

dropped in the array on the line above, or to the right...

 

So I am having a devil of a job laying out my final array or LED's

according to an exact alignment as the components are off some fraction

of my grid that I can't adjust for (even with the fine grid set very

fine), and anyway that is now extremely time consuming (imaging 1000

LED's that all need to be manually aligned rather than snapping to an

exact grid.

 

Is there a fix for this initial automatic grid when initially creating a

PCB to work on ?

 

Any help or ULP's to fix this would be appreciated...

 

I even took a look at editing the .brd XML file and while is looks

possible it is too daunting of a task and possibly more manual and

probably error prone.

To clarify, the schematic is drawn with the standard 0.1" grid, but when

creating the board a default 0.05" grid is used to drop all of my

componenets onto in an array to the side of the default PCB area, but

row to row and column to column placements are off once the placement

grid is set to my 1mm grid by fractions of a mm but its enoght o make

final placement of the components impossible without setting a

ridiculously fine alternate grid setting.

there must be a way to make eagle default to a metric grid on the PCB

layer before it has already dropped all my components on there for me to

then place.

AARGH..

I'm not sure I understand the problem, but I'll try to help...

The array on the left side is merely a holding area, a temporary place for

all the parts.  As far as I know, there is no way to control that area at

all.  The parts are all placed there in order by part type.

You can set the grid to anything you want (set your defaults in eagle.scr),

and then move each part from the temporary area into your board outline.

As far as I know, the usual procedure is to grab one part at a time and

move it to the board.  Are you trying to move a group of parts all at the

same time?

You can see a thread with some thoughts about how I've dealt with this at:

http://www.element14.com/community/thread/31802/

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

Am 31.08.2014 um 01:21 schrieb peter:

On 08/30/2014 03:54 PM, peter wrote:

I'm using Eagle Pro 6.6.

 

I noticed a behaviour that has me very frustrated and I can't find a way

to fix it.

 

If I create a Schematic with say 64 LED's (SMD devices to created with a

grid on 0.1mm in the library)

 

And wire them up appropriately in the schematic.

 

then switch to the PCB view, the 64 LED's are automatically placed on

the board outside of the default PCB area, but they are placed in a n

array  pattern that i have no control over, and that seems to be

slightly off when I then set the PB grid to 0.1mm for placement...

 

from row to row of LED's they are slightly misaligned when i pick them

up to place them they don't line up correctly with LED's that were

dropped in the array on the line above, or to the right...

 

So I am having a devil of a job laying out my final array or LED's

according to an exact alignment as the components are off some fraction

of my grid that I can't adjust for (even with the fine grid set very

fine), and anyway that is now extremely time consuming (imaging 1000

LED's that all need to be manually aligned rather than snapping to an

exact grid.

 

Is there a fix for this initial automatic grid when initially creating a

PCB to work on ?

 

Any help or ULP's to fix this would be appreciated...

 

I even took a look at editing the .brd XML file and while is looks

possible it is too daunting of a task and possibly more manual and

probably error prone.

 

To clarify, the schematic is drawn with the standard 0.1" grid, but when

creating the board a default 0.05" grid is used to drop all of my

componenets onto in an array to the side of the default PCB area, but

row to row and column to column placements are off once the placement

grid is set to my 1mm grid by fractions of a mm but its enoght o make

final placement of the components impossible without setting a

ridiculously fine alternate grid setting.

 

there must be a way to make eagle default to a metric grid on the PCB

layer before it has already dropped all my components on there for me to

then place.

 

AARGH..

Well inch is not millimetres

So if you use devices with fractions of millimetres spacing why don't

you set the grid appropriate? You can set it to microns, mils, inch and

millimetres and if you want a default setting you can do that in the

eagle.scr file.

Help grid.

--

Mit freundlichen Grüßen / With best regards

Joern Paschedag

On 31/08/14 00:21, peter wrote:

 

To clarify, the schematic is drawn with the standard 0.1" grid, but when

creating the board a default 0.05" grid is used to drop all of my

componenets onto in an array to the side of the default PCB area, but

row to row and column to column placements are off once the placement

grid is set to my 1mm grid by fractions of a mm but its enoght o make

final placement of the components impossible without setting a

ridiculously fine alternate grid setting.

 

there must be a way to make eagle default to a metric grid on the PCB

layer before it has already dropped all my components on there for me to

then place.

 

AARGH..

As Doug said, the initial placement of parts on the blank board is

merely a holding area. They're just dumped there with no attempt to

psychically second-guess your actual desires. The use of a 0.05" grid is

the default and makes a lot of sense because even these days most

components are actually built to an imperial grid.

When moving the LEDs to where you want them, you will need to place them

on your preferred grid. Press the  key when you pick them up to

move them. This does a "snap-to-grid" using the grid you currently have set.

Alternatively, place them using the command line, where precise

coordinates can be entered. Or write a script to do so, or a ULP (or

Python program or whatever) to auto-generate said script.

HTH

Rob

peter wrote on Sat, 30 August 2014 18:54

Is there a fix for this initial automatic grid when initially creating

a PCB to work on ?

By mentioning "fix", you imply there is anything wrong with how it works

now.  There isn't.  There is no reason to care where exactly unplaced part

are initially put off-board, since they are, well, unplaced.

Normally you wouldn't even have the sea of unplaced parts in view when

doing placement.  All that matters is that they are out there somewhere.

As you walk thru the schematic (I print it out, then cross off parts as I

place them) to place parts on the board, you enter the part name and it

shows up at the cursor.  Wherever it was previous to that is completely

irrelevant.

However, when you have a regular array of parts to place, you wouldn't do

this manually anyway.  That would be too slow, tedius, and unreliable.

Write a program that generates the script to place the array of parts, then

run the script.  The original positions of all the placed parts is

irrelevant.  If there is a error in the script or you want to change

something, you regenerate and rerun the script.  The parts will show up in

their new positions, this time even though they were previously placed on

the board.  Again, the previous positions of the parts doesn't matter.

There is no problem here, so nothing to fix.

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

On 31/08/2014 10:54 a.m., peter wrote:

I'm using Eagle Pro 6.6.

 

I noticed a behaviour that has me very frustrated and I can't find a way

to fix it.

 

If I create a Schematic with say 64 LED's (SMD devices to created with a

grid on 0.1mm in the library)

 

And wire them up appropriately in the schematic.

 

then switch to the PCB view, the 64 LED's are automatically placed on

the board outside of the default PCB area, but they are placed in a n

array  pattern that i have no control over, and that seems to be

slightly off when I then set the PB grid to 0.1mm for placement...

 

from row to row of LED's they are slightly misaligned when i pick them

up to place them they don't line up correctly with LED's that were

dropped in the array on the line above, or to the right...

 

So I am having a devil of a job laying out my final array or LED's

according to an exact alignment as the components are off some fraction

of my grid that I can't adjust for (even with the fine grid set very

fine), and anyway that is now extremely time consuming (imaging 1000

LED's that all need to be manually aligned rather than snapping to an

exact grid.

 

Is there a fix for this initial automatic grid when initially creating a

PCB to work on ?

When you create a board from a schematic the board is created with the

default grid and the packages are initially on that grid. Then if you

change the grid to what you want, the packages don't adjust their

position so they are 'off grid' at that time.

There is a ULP you could run before you start to layout which will move

all your packages onto your nominated grid. Have a look at cmd-snap-brd.ulp

HTH

Warren

On 08/30/2014 10:45 PM, Joern Paschedag wrote:

Am 31.08.2014 um 01:21 schrieb peter:

On 08/30/2014 03:54 PM, peter wrote:

I'm using Eagle Pro 6.6.

 

I noticed a behaviour that has me very frustrated and I can't find a way

to fix it.

 

If I create a Schematic with say 64 LED's (SMD devices to created with a

grid on 0.1mm in the library)

 

And wire them up appropriately in the schematic.

 

then switch to the PCB view, the 64 LED's are automatically placed on

the board outside of the default PCB area, but they are placed in a n

array  pattern that i have no control over, and that seems to be

slightly off when I then set the PB grid to 0.1mm for placement...

 

from row to row of LED's they are slightly misaligned when i pick them

up to place them they don't line up correctly with LED's that were

dropped in the array on the line above, or to the right...

 

So I am having a devil of a job laying out my final array or LED's

according to an exact alignment as the components are off some fraction

of my grid that I can't adjust for (even with the fine grid set very

fine), and anyway that is now extremely time consuming (imaging 1000

LED's that all need to be manually aligned rather than snapping to an

exact grid.

 

Is there a fix for this initial automatic grid when initially creating a

PCB to work on ?

 

Any help or ULP's to fix this would be appreciated...

 

I even took a look at editing the .brd XML file and while is looks

possible it is too daunting of a task and possibly more manual and

probably error prone.

 

To clarify, the schematic is drawn with the standard 0.1" grid, but when

creating the board a default 0.05" grid is used to drop all of my

componenets onto in an array to the side of the default PCB area, but

row to row and column to column placements are off once the placement

grid is set to my 1mm grid by fractions of a mm but its enoght o make

final placement of the components impossible without setting a

ridiculously fine alternate grid setting.

 

there must be a way to make eagle default to a metric grid on the PCB

layer before it has already dropped all my components on there for me to

then place.

 

AARGH..

 

Well inch is not millimetres

So if you use devices with fractions of millimetres spacing why don't

you set the grid appropriate? You can set it to microns, mils, inch and

millimetres and if you want a default setting you can do that in the

eagle.scr file.

Help grid.

 

 

It is difficult to explain .. but try it and you'll see... build a

simple schematic with say 40 SMD LED's (use an LED designed on a mm

based grid) and then move to a board to start laying the PCB..

now if you have a default eagle.scr file it will have placed those

components in a board with a default 0.1" grid and will have dropped

them in an array (based on that 0.1" grid) to the side of the board...

now if you change the grid to the mm grid that is best for the LED's you

will note that as you try to pick up and place them in a mm based grid,

the LED's from the first row will not align perfectly with the LED's

from the second row, or the third row... etc... even with very very fine

alternate grid spacing its all but impossible to  get them to align

perfectly (and this defeats the purpose of having a grid anyway, since

that is supposed to help with rapid aligned placement of devices)

On 08/31/2014 04:48 AM, Olin Lathrop wrote:

peter wrote on Sat, 30 August 2014 18:54

Is there a fix for this initial automatic grid when initially creating

a PCB to work on ?

 

By mentioning "fix", you imply there is anything wrong with how it works

now.  There isn't.  There is no reason to care where exactly unplaced part

are initially put off-board, since they are, well, unplaced.

yes and no. yes they are 'unplaced' but they are unplaced according to a

grid that is derived from the defaults set up in the eagle.scr file.

once they have been 'unplaced' they are tied to a position relative to

the grid (initially they are on a 0.1" grid), but if I change to a 1mm

grid they now obtain a new relative position according to their current

position off the 1mm grid, and when moved they will maintain that offset

from the 1mm grid, getting them back onto the 1mm grid is what I'm

struggling with.

 

Normally you wouldn't even have the sea of unplaced parts in view when

doing placement.  All that matters is that they are out there somewhere.

As you walk thru the schematic (I print it out, then cross off parts as I

place them) to place parts on the board, you enter the part name and it

shows up at the cursor.  Wherever it was previous to that is completely

irrelevant.

 

I have not delved into writing ULPs yet... one day when i have time.

However, when you have a regular array of parts to place, you wouldn't do

this manually anyway.  That would be too slow, tedius, and unreliable.

Write a program that generates the script to place the array of parts, then

run the script.  The original positions of all the placed parts is

irrelevant.  If there is a error in the script or you want to change

something, you regenerate and rerun the script.  The parts will show up in

their new positions, this time even though they were previously placed on

the board.  Again, the previous positions of the parts doesn't matter.

 

There is no problem here, so nothing to fix.

 

peter wrote on Mon, 01 September 2014 04:56

It is difficult to explain

Actually it's quite clear what Eagle is doing.  The part that makes no

sense is why this should be a problem.

Quote:

build a simple schematic with say 40 SMD LED's (use an LED designed on

a mm based grid) and then move to a board to start laying the PCB..  now

if you have a default eagle.scr file it will have placed those components

in a board with a default 0.1" grid and will have dropped

them in an array (based on that 0.1" grid) to the side of the board...

OK

Quote:

now if you change the grid to the mm grid that is best for the LED's

you will note that as you try to pick up and place them in a mm based

grid, the LED's from the first row will not align perfectly with the

LED's

This is what makes no sense for at least three obvious reasons.

First, by "pick up" it seems you are trying to drag the parts onto the

board individually.  Clearly you want to make a script to place a array of

40 parts.

Second, even for individual parts, dragging them from off the board doesn't

make sense.  It is slow and tedius because it requires more mouse usage,

you have to zoom back to see the board and the whole off-board holding area

for the parts, and it can be quite difficult to find a small part in the

holding area.  With the MOVE command, you can keep the view zoomed into the

small area of the board you are currently working on, you enter the

designator directly without having to hunt for the part, and the original

grid doesn't matter.  The part just appears at the cursor from "someplace".

You don't need to know nor care where that someplace is.  Since this is

done a lot during placement, I have F12 set up for 'ratsnest; move'.  Note

no semicolon after MOVE.  That doesn't end the command so that I can type

the part designator parameter.  To place a part, I hit F12 type the

designator, and hit ENTER.  Poof, the part appears at the cursor much

faster than someone go over to the part holding area hunt around for it and

drag it back to where they're working, probably requiring some more panning

and zooming.

Third, even if you want to do it the slow and tedius way, CTRL lets you

pick up the part at its origin regardless how it might be snapped to the

grid.  Didn't you read the help on MOVE at all!!?

You should at least learn the tool before complaining about it.

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

peter wrote on Mon, 01 September 2014 05:05

 

Normally you wouldn't even have the sea of unplaced parts in view

when

doing placement.  All that matters is that they are out there

somewhere.

As you walk thru the schematic (I print it out, then cross off

parts as I

place them) to place parts on the board, you enter the part name

and it

shows up at the cursor.  Wherever it was previous to that is

completely

irrelevant.

 

I have not delved into writing ULPs yet... one day when i have time.

Huh?  What does anything I mentioned there have to do with ULPs?  Read what

I wrote.  This is just using Eagle commands normally.

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.