Component Placement from file

[mngojuce]

Hello, I have a very large number of components that need to be arranged in a very specific pattern. I'm using Altium 17 and I see that it has an option to perform component placement from a file. I've done some research and it seems I can take the exported pick and place file from an existing project (where I have these components arranged in a grid and employ the same origin), change the center locations of the components I want to the new locations, change the extension to .PIK, and select the file. However, doing this on 5 components, as a test, it seems as if those components get deleted or placed in no man's land. Anyone have experience with using the "Place from file" feature in Altium. What format does this file need to be in, how do I generate it, and what information does it need? Thanks in advance!

[s.gesota]

Actually you can just copy paste that particular component from the previously completed project to the current one, I do it for my designs too.I haven't faced any issue with this copy pasting component. However i don't have any information about the "Place From File". Simply copy pasting from previous sheets has always worked for me. ( I use Altium 16) [This might help you for SCH design and NOT THE LAYOUT]

[mngojuce]

Yep, I've done that in the past too and that works if I want them in the same spots again. In this case, I need to place a very large number of components (same ones and over 200) in very specific and new locations as defined by a coordinate file and instead of manually placing them by hand the Place from file option would save me a lot of time. A random example would be my existing project has the components in a square grid and new one has them arranged as many small triangles.

[robertferanec]

I have never done this. Please let us know how you solved the problem. Thank you.

[mngojuce]

Turns out you can use PCB List (In Altium on bottom right choose PCB->PCB List or on keyboard V->W->P->L) to do this. Copy the info to Excel by right clicking the selection and select "Copy with Header". I selected the entire row just to be safe. Open Excel and paste info into an empty spreadsheet. Make the changes required in Excel. For me it was easy because I had a coordinate file with all the XY center coordinates (X1 and Y1). Copy all the new info into Excel including the header. Then in PCB List right click on the selected rows and select "Smart Grid Paste". In the pop-up box verify the Header Row is selected (top right) and in my case I had to hit the "Choose Visible Columns" button to show X1 and Y1 so I can verify updates were made. Top panel shows the changes copied from Excel. Finally, hit the "Automatically Determine Paste" button, double check updates were made (bottom panel and bold), and then the OK button. Close PCB list, updates should have been made.

[robertferanec]

Thank you so much mngojuce

[MikeS]

It may help to know that a website Surface Mount Process offer the service to create component placement files from Gerber data - http://www.surfacemountprocess.com/c...n-service.html

[Tom Yunghans]

I created a pick and place file using "File/Assembly Outputs/Generate Pick and Place Files" which could then be used without error when using it with the "Tools/Component Placement/Place From File" command. However, I wanted to modify the positions of the components with positional information from another spreadsheet. I first read the pick and place file (text file) into Excel. I had a hard time getting the fields right, but thought I was successful. I then did some sorting on the excel file and then some copy/pasting of the positional information from one spreadsheet to another. I then tried to generate a new pick and place (text) file from the modified spreadsheet, but could never seem to get a file which Altium didn't complain about when I tried to read it into the design using "Tools/Component Placement/Place from File. Altium documentation is very sparse on the format requirements for the pick and place file, and the Altium forum solutions recommended by various individuals didn't seem to work for me either.

I finally gave up and used the approach using the "PCB List" mentioned above.