[SOLVED]How to move a group to a defined location in EAGLE? - Page 1
Forum section: electronics / general

author: jpanhalt
author_rank: Super Contributor
timestamp: June 07, 2016, 09:08:49 pm
content: I was moved to post a new thread by comments in this thread:https://www.eevblog.com/forum/chat/why-is-eagle-cad-soft-so-painful-to-use/msg955599/#msg955599I have used EAGLE from V.3.xx as a hobbyist and am pretty comfortable with it. Nevertheless, when I have critical dimensions for a board outline, I make the outline in my favorite CAD program and import it as a DXF into EAGLE. I don't like to get "just close," with a mouse, so I align a "zero point" on my imported DXF with the zero point for the EAGLE board. I also use the command line freely.However, for aligning the import, I still rely a manual "kludge" -- if that is the correct term. It is doable, but not elegant.Is there any way to define a group's alignment point (coordinate) and move that to a new coordinate (e.g., 0,0) with the command line?Regards, John

author: MarkF
author_rank: Super Contributor
timestamp: June 07, 2016, 09:14:24 pm
content: Another reason I use DipTrace. I can place components with the mouse or enter exact x,y locations from the keyboard. Keyboard entry is available for board size, component placement, pad size, copper pour points, etc.

author: jpanhalt
author_rank: Super Contributor
timestamp: June 07, 2016, 09:24:57 pm
content: I can do the same with components in EAGLE quite easily. There is even a ULP to align all components simultaneously.I am talking about a GROUP of components that is imported.John

author: MarkF
author_rank: Super Contributor
timestamp: June 07, 2016, 09:53:12 pm
content: DipTrace can group components and treat them as one unit.

author: jpanhalt
author_rank: Super Contributor
timestamp: June 07, 2016, 10:14:27 pm
content: Does it allow you to define the "origin" of the group and then move that origin via commands to a specific spot? EAGLE treats a group as a single entity.John

author: Jeroen3
author_rank: Super Contributor
timestamp: June 08, 2016, 07:30:00 am
content: Put the board outline in the PCB as a footprint using ADD. It will then get an origin and appear as inseparable group. You'll have to draw it as footprint first. But that should be obvious.Easy re-using as well.

author: MarkF
author_rank: Super Contributor
timestamp: June 08, 2016, 10:27:16 am
content: Quote from: jpanhalt on June 07, 2016, 10:14:27 pmThe origin is the center of all the objects grouped together. After that, the group is treated as a single entity and you can specify the location via the keyboard or rotate the group or just drag it with the mouse.

author: jpanhalt
author_rank: Super Contributor
timestamp: June 08, 2016, 02:59:15 pm
content: QuoteOn my version of Eagle 7.2.0, it does not seem to behave like that. Here is a dxf file that was imported into Eagle. The rectangle is 2"x3" and the alignment mark with circle is in dead center. Note that the Y-axis of the center of the imported file (dimension layer) is nowhere near the origin of the drawing plane (0.5" grid shown so the error is more evident). Moreover, looking at propertires, the offset is not some simple multiple of the grid.Also, I have not figured out how to move the entire group a specified amount using the command line. Simply being able to do that would make it a lot easier to align. What is the command line "command" to control the whole group?John

author: MarkL
author_rank: Unknown
timestamp: June 08, 2016, 04:02:51 pm
content: You could:- Group the imported rectangle and center mark;- Move it as a group with the offset needed to make your alignment land on drawing (0,0). In this case, to the right and down:move (c>0 0) (0.21875 -0.21875);Another option is to temporarily redefine the grid to be spaced at 0.21875 intervals, drag the group one interval right and down, and then put the grid back.EDIT: An easy way to put the grid back is to right-click on the grid icon. There's a "Last" option. You can also define an alias from the right-click menu for the 0.21875 grid setting, if that's a recurring number.

author: MarkF
author_rank: Super Contributor
timestamp: June 08, 2016, 04:03:24 pm
content: Do a quick download of the free version of DipTrace and see if it performs like you want. The limits of the free version are 300 pins and 2 sides.It''s also easy to import your Eagle schematic and PCB layout into DiipTrace.

author: jpanhalt
author_rank: Super Contributor
timestamp: June 08, 2016, 04:25:40 pm
content: Quote from: MarkL on June 08, 2016, 04:02:51 pmThat was the trick. BTW, the alternative is what I have been doing ever since I started importing dxf's. It works, but as I mentioned, it was a workaround.Thank you both.John