Adding custom shape to top copper layer

[NFrank89]

Hello all!
I am trying to add a custom shape to the top copper layer of my PCB and would like to know the best way to achieve my desired result.
This is the shape and it must have a radius of 3.175mm. The closed sections (upper left and lower right) must be solid copper filled.


How would you recommend going about this?

Thanks!

[Tomg]

1) Draw the shape outline (no fill) in your favorite 2D CAD program and save it as a DXF file.
2) Open your board file, select File in the Main Menu, choose Import in the drop-down menu and click on DXF... in the fly-out menu.
3) In the Open dialog window navigate to and select/highlight the DXF file and click on the [Open] button.
4) In the Import DXF dialog window, use the settings shown in the illustration below and click on the Import button.

[NFrank89]

Thanks for the response, Tom!
I'll have to see if I can do this in solidworks.
Would you mind sharing the file you came up with for the example?

[Tomg]

Here you go (it's inside the zip folder named "copper.zip" below)...

[NFrank89]

Great! Thank you so much!

-- 20 Jun 2017, 08:49 --

What is the best method for accurately placing these targets so that the center point is .240 from the left edge of the board and 1.25 from the bottom? Coming from SolidWorks, I am used to placing a part in the workspace then simply adding dimensions to accurately locate the part and lock it in place. I am ripping my hair out trying to place things in the PCB editor, it is absolutely maddening having to change the grid size or entering the x/y coordinates for each individual point of a line or object. I often find that if I am having too much trouble I must be doing something wrong. Can you help me understand placement better?

[Tomg]

Unfortunately, DipTrace does not have a parametric environment so you will not be able to move objects around by assigning dimensions. DipTrace dimensions do not do the driving; they are "passive" and are driven by the objects they measure. To move a component (other than dragging it with the mouse), click on it to select it and enter new coordinate values (X,Y) in the Properties panel on the upper-right side of the screen. An alternate method would be to right-click on the component (not its pads), choose Properties... in the pop-up menu and enter the desired X and Y values in the lower-left side of the Component Properties dialog window. Component coordinates specify the location of the component's origin. To view a component's origin, right-click on it (not its pads), select Pattern Origin in the pop-up menu and choose Show in the fly-out menu. The component origin will appear as a small gray "+".

Since the imported copper object is not a singular "component", you will have to move it by changing the grid size, selecting/highlighting the desired object(s) and then using the arrow keys. Notice that I centered the copper object(s) around my CAD program's origin (0,0) when creating the drawing. This means that it should import into the DipTrace Design Area at the same location (0,0) as long as your version of DipTrace is not too old. The following procedure is one way to work with different grid sizes and it might introduce to you one particular grid feature you may not have been aware of...
1) Enter a grid size of 0.24mm at the top of the screen.
2) Select View in the Main Menu, choose Y Grid Size in the drop-down menu, click on Custom... in the fly-out menu, enter 1.25mm in the Grid Size dialog window and select OK.
3) Select/highlight the imported object(s).
4) Press the right-arrow key once. This should move it to the right 0.24mm.
5) Press the up-arrow key once. This should move it up 1.25mm. The center of the imported object(s) should now be located at (0.24,1.25).
6) To reset the grid back to the normal X/Y ratio, select View in the Main Menu, choose Y Grid Size in the drop-down menu and click on Identical with X in the fly-out menu.

Another way to move the special object around would be to import it into the pattern editor instead and save it as a new "pattern". Then place the new "pattern" into the PCB layout, give it the desired coordinates and perform an "Ungroup Component" on it to turn it back into an ordinary copper object.

I hope this helps ease some of the pain.

[NFrank89]

You sir, are a gentleman and a scholar!

That made this so much easier. thank you for introducing me to the "Y grid size" option!