I am trying to create an assembly drawing for a large (.44" x 26.25") board. The board is routed and has been sent to the shop for fabrication and turnkey assembly. Although the shop did not specifically ask for an assembly drawing, I need to make one per contract. I am trying to do this by exporting to .DXF and finishing the drawing in Acad.
This seems to be a tricky task. The export works, but creates a separate .dxf drawing for each layer. There appears to be no easy way to select what shows up on the drawings. The pcbnew file looks like the first screen shot. This is what I would like the assembly drawing to look like. In pcbnew you are free to select layers. The other shot shows two of the dxf files.
===== how to load screen shots??? =====
There has to be a better way. I think I will need to merge some of the dxf drawings and superimpose to get both the tracks, pads, and fab layer details, not sure how hard this will be. The other issue is the files are exported at about 25x scale, so they all need to be re-scaled in Autocad. Also I can’t seem to turn off the component values when I export, this really clutters things up.
I create assembly drawings straight of Pcbnew in Kicad using the print dialog saved as a PDF for turnkey assembly. What information are you looking to place on your assembly drawing?
I typicaly create three PDFs:
README.PDF
Top Silkscreen
Top and Bottom Copper
Comments layer is shown with the following:
Layer Stackup with Filename extension callouts
Board thickness
Board material
Board finish
Board Silkscreen & Mash
Controlled Impedance Callouts, matching Net Names
TOP_ASSEMBLY.PDF
Board dimension callouts on Drawings layer
Top Silkscreen shown
Top Courtyard Shown
Top Fab Shown
(Between the Silkscreen, Courtyard and Fab layers the assembly house should easily see the location and rotation of every part)
BOTTOM_ASSEMBLY.PDF
Same as TOP ASSEMBLY, but only bottom Silk, Courtyard, and Fab. This is also printed to PDF ‘Mirrored’ to match looking at back of the actual board.
Double apologies- this thread should have been in ‘manufacturing’. Also the obvious eluded me, I was looking for ‘attach’ or ‘screenshot’, ‘upload’ should have been a clue.
The top shot is what I would like the assembly drawing to look like- this is directly from pcbnew. The bottom shots are the dxf files after import into acad and resizing. Left one is front fab, right is front cu. I was hoping to edit and superimpose these to create the assembly dwg. BUT- a) can’t get the partnames out of the fab, b) (it’s hard to see) the text is all in double lines, graphic lines not text so I can’t edit, c) having trouble with display order, i.e if I add hand drawn parts, I want them to be on top & obscure the bottom (this is an autocad issue, still researching).
So all told this is a pain. Why not use the plot-to-pdf direct from pcbnew? This is a bizarre board, dimensions 0.44 x 26.25". To show adequate detail I think this needs to go on a ‘D’ size drawing at 1:1, so I’m trying to use acad. If I plot this to an A sized pdf the details are lost. There is probably a workaround, but I’m not too familiar with graphic programs, you may be able to save a pdf to a D-sized drawing(??).
Thank you Aaron for the pdf suggestions. At this point the shop is content to turnkey without a pcb fab (drill and trim) or top level assembly. I just need these to fulfill contract obligations. The pcb fab is done, that was a simple import via dxf and edit with notes and title block. The top level assy is what I am working on now.
I use PDF Creator (there is a free version) on windows to print to PDF files. There are many other programs out there, of course. If I select this as my printer in the print dialog, I can print to ANSI D paper size as a PDF:
I have a template with title block and assembly notes. It’s important to understand the comment, drawing and fab layers, especially when making footprints, so you can create a clean assembly drawing. I try to do everything in Kicad if I can to avoid the extra third party tool editing.
Noticed that Q10 silkscreen and pin numbers do not line up. Silkscreen indicates pin 1 over the net of pad 3.
Note that the device package changes the pin number assignment. If this was breadboarded with leaded parts, then the pin assignments are likely incorrect for a SMD part.
Pin 1 G, Pin 2 S, Pin 3 D - Typical for SOT-23 transistors.
I’m having a similar issue.
What I have done, at the moment, is to draw the outlines on the Fab layer. This is very time consuming. However, this only needs to be once, and there are some tricks to make the effort go faster.
When I plot, I plot to PDF. However, in doing this, only one layer shows up on each individual Gerber. I thought about using GerbV to view the layers… Wait, let me do that!
Here is KiCad view of a section of Pcb showing Silkscreen layer:
Obviously there are some collisions between the layers as I did not have the method sorted out yet.
Like I said, it seems a lot of work to draw the physical parts, but I knew I wanted to create an assembly drawing with good details. I just had not worked through the entire process.
Using GerbV to Export both layers to a single PDF:
Good catch Sprig! This is a prime example of how not fixing something early propagates. I originally had the symbol and footprint wrong for the particular part. Rather than fixing it I just shuffled the pins around. Although electrically correct and routed, now I find that all the fab layer parts are reversed too. Although confusing, I let it go since this is a 3-pin part that can only go in one way. I will probably edit the footprint to put the notch in the right corner, then update the part.
I like the idea of spending time up front on the fab layer. Also some posters have recommended editing part fields with BOM items like cost, second source, etc. More work early but makes BOM and XY position files easier later on.
I have for now abandoned the pdf route, although it has promise. Ultimately I will need to deliver a .dwg or .dxf drawing to the client, so if I were to do the pdf then I’d have to re-convert it. The acad assembly drawing is proving very tedious but doable. I will need to make ‘blocks’ for the parts and place them on the copper layer. To fix the case where things need to be covered by the part I am using crosshatching. Sadly I will also have to type in all of the ref des text, the fab layer stuff is lines rather than text, unsuitable. This will be a rather bizarre assy drawing! I hope this is a one-off (because of the large size), and that in the future I can take the pdf approach.
