I needed to place connectors for another board in a specific place of my board. I have the original board drawing with dimensions.
First I used the dimension tool. It allows only very, very imprecise dimension drawing, up to the accuracy of the grid. So I set the grid to 0.01mm and finally made it. When the dimension length is set - it cannot be reset. Or can it? I couldn’t find any tool for that. There are “precise move” options, but they work to precisely move the imprecisely drawn dimension. This is pretty crazy. The normal flow would be just to type the exact dimension I have in my documentation. I can type my dimension, but this won’t change the real dimension but create a fake dimension! Does anyone use such function at all? What’s the use of this tool?
Another thing: the dimensions are drawn on my copper layer. I don’t want them there. I want them on any other supportive layer, I use them only to position my connectors correctly. I see no option to move them to another layer. I suppose I just need to delete them.
It seems like the tool is designed for something completely different than positioning the elements precisely, because it seems like every possible effort was made to make it as difficult as possible.
Here’s the board I take the dimensions from. It’s the ST-MOD connectors, 4 of them, they must be perfectly aligned with my board otherwise I won’t be able to connect boards with each other. I finally placed the connectors perfectly, but I wonder that maybe I’m doing it completely wrong and there is an easier, proper way of doing that.
It seems like the tool is designed for something completely different than positioning the elements precisely
Thats correctly identified. The main use of the dimension-tool is to produce dimension-drawings (like in your picture from the board).
Another thing: the dimensions are drawn on my copper layer. I don’t want them there. I want them on any other supportive layer, I use them only to position my connectors correctly. I see no option to move them to another layer.
Set the layer you want before you draw the dimension-item. Or if you want to change the dimension-layer afterwards: doubleclick the dimension-item → you get the dimension-properties-dialog–> change the layer-setting in this dialog.
If you want to precisely position some footprint/hole/…: doubleclick the item -->the property dialog opens → normally there are fields for x/y-coordinates so you can fill in the desired position.
If you want to position one item in respect to another item:
place both items at the same position (exactly on top of each other)
select the item you want to move away
use the already discovered “Move exactly”-tool
If you afterwards want to check if the position is good: try also the Inspect–>Measure tool. This is interactively and doesn’t produces a dimension-number on the board - useful for dimension-checking.
A procedure I often use for exact placement is using dx & dy.
In this instance I wanted the center of pin 9, top IC, exactly 315 mil in and 335 mil down from the edge cut corner. I then wanted the centre of pin 1, lower IC, exactly 400 mil below the pin 9.
To do this I set a suitable grid (5 mil).
Placed the mouse on the edge cut corner.
Tapped the space bar, which set dx & dy to zero.
Moved the mouse to the centre of pin 9.
Tapped the M key which grabbed the footprint by the center of pin 9 and moved that footprint while I watched the dx & dy readouts.
When dx = 315 mil & dy = 335 mil I tapped the enter key.
I then repeated the performance for the lower footprint, but this time I first placed the mouse on pin 9 of the upper IC.
Tapped the space bar (which zeroed dx & dy again).
Placed the mouse in the centre of pin 1 lower IC, and tapped M.
Read dx & dy as I moved the mouse holding pin 1 so the reading was dx = 0 and dy = 715.
tapped the enter key… all done.
Note: Full window cross hairs for the mouse help when doing this.
I suggest using a 3rd party cad design software and exporting it as dxf. Or you FreeCAD with StepUp addon workbench which can export a KiCad layer directly from a constrained Scetch. Are there 4 mounting holes in the corners? They would belong in the Edge.Cuts layer together with the outline. You can draw the Edge.Cuts layer separately and then another drawing to help for locating components, or you could draw everything in one helper layer. Draw a smallish circle centered on each strategic location (connector pin which needs to be placed exactly).
When you have the footprint and corresponding helper circle in the KiCad board, select a pad of the footprint. Open the context menu → Special Tools → Position Relative to. In the dialog click Select Item, then select the circle on the board. Again in the dialog set the offset to 0 and accept. Now the footprint should be located so that the pad is in the center of the circle.
This kind of moving may require certain settings; if you try this and have problems, please ask. The pad anchor must also be in the center of the pad because your technical drawing seems to be designed that way.
