Through Hole Pad without Drilled Hole

Making PCB Layouts, Manual routing, Auto-routing, Copper pouring, Updating from Schematic, Manufacturing Output
Post Reply
Message
Author
SteveW
Posts: 14
Joined: 05 Oct 2019, 18:49

Through Hole Pad without Drilled Hole

#1 Post by SteveW » 20 Sep 2021, 15:23

I need to provide UNDRILLED corner pads at the four corners of a single sided PCB. They will not be connected to anything, just isolated pads on just the bottom side copper. I WOULD like them included Is there an easy way to convert a standard round pad to keep the drill specification out of it? I do not want a filled circle, but rather a round pad with a drill hole LOCATION present for future drilling of corner holes. Do I have to go into Pattern Editor and "roll my own"? Not sure I even know how I would do that. And I suppose I could always edit the NC Drill file and just remove those 4 lines, but hoping there is and easy way in Diptrace. Thanks.

Tomg
Expert
Posts: 1773
Joined: 20 Jun 2015, 14:39

Re: Through Hole Pad without Drilled Hole

#2 Post by Tomg » 21 Sep 2021, 13:41

Do I have to go into Pattern Editor and "roll my own"?
Yes.

The ability to make a pad with a copper void has been submitted as a feature request in the past, but so far nothing has come of it. The workaround involves creating a DXF drawing/file with two concentric circles of the desired dimensions where the outer circle represents the pad diameter and the inner circle represents the copper void. You can use a competent 2D CAD program to accomplish this and then skip to step 5 below. The alternative is to use DipTrace to create the DXF file by first following steps 1 through 4 before continuing on to step 5...

Creating the DXF file using Diptrace
1) Open a new/blank instance of the PCB Layout editor and draw the two circles (obrounds) centered about the origin on the Top Assembly layer. Please note that this is the only place where the dimensions can be set.
2) In the main menu select "File" > "Export" > "DXF..." to bring up the "Export DXF" dialog window.
3) In the "Export DXF" dialog window select/highlight the "Top Assembly" layer, choose the desired units using the "Units:" drop-list, enable the "[x]Use Design Origin" option, click on the "[Export]" button to bring up the "Save As" dialog window and save the new DXF file to a convenient location (e.g the Desktop).
4) Close the current PCB Layout editor instance without saving the board file that contains the two circles.

Importing the DXF file into the Pattern Editor
5) In the Pattern Editor choose the "User Patterns" group, select/highlight the desired target library and add a new pattern to it using the hotkey combination "[Ctrl]" + "[Insert]". A new blank pattern named "Untitled" should appear in the patterns list on the left side of the screen. Make sure it is selected/highlighted, then give it a new name before proceeding to the next step.
6) In the main menu select "Pattern" > "Import from DXF..." to bring up the "Open" dialog window.
7) In the "Open" dialog window locate and select/highlight the new DXF file and click on the "[Open]" button to bring up the "Import DXF" dialog window.
8) In the "Import DXF" dialog window set "DXF Units:" to match that of the DXF file, set "Import Mode:" to "Add", click on the "Top_Assembly" layer in the "Layers" list, set "Convert to:" to "Top Signal", enable the "[x]Fill Closed Areas" and "[x]Embedded Polygons" options and click on the "[Import]" button. A new filled drawing figure with a center copper void should appear in the Design Area.
9) Right-click on the outside edge of the new drawing figure and select "Convert to Pad" in the context menu.
10) Create a copy of the new pad (make sure pad numbers don't repeat) and place it next to, but not touching, the original.***
11) Resave the pattern library using the hotkey combination "[Ctrl]" + "s". The new pad "pattern" is now ready to use in the PCB layout.

***Note: The second pad is needed for DipTrace to recognize the new pattern as a "smashable" component when it is placed on a PCB. The pattern's "component" state is temporary. After it is placed on a PCB right-click on it (not directly on one of the pads - move the mouse around and look for the green highlight) and select "Ungroup Component" in the context menu so that it will revert to being recognized only as two independent polygonal surface mount pads without reference designators. Because it is no longer a "component" the BOM tool will not list it. The new independent pads can be copied as many times as needed and moving them is possible using mouse-dragging and/or coordinate entry techniques. Since the pads are polygons their size cannot be altered on the PCB. Any size changes must be applied while creating the original drawing for the DXF file.
donut_3D.png
You do not have the required permissions to view the files attached to this post.
Tom

SteveW
Posts: 14
Joined: 05 Oct 2019, 18:49

Re: Through Hole Pad without Drilled Hole

#3 Post by SteveW » 21 Sep 2021, 14:34

Hi Tom,
OK, I can do that, I think. I use Corel for most of my artwork and it exports DXF pretty well...... most of the time. I really appreciate how much time you spend responding to all of us. Another suggestion I found back a few years was to just make a circle of the right size then expand its line width in properties. I played with that at home, and with a bit of fiddling, got the right ID and OD, but couldn't figure out how to move it to the bottom copper layer where I want it. Being as new at this as I am, I am sure I was just overlooking something obvious. Maybe you can answer another question for me: on these simple single sided boards I am drawing, I do want a solid fill mask on the top side under the silk screen to enhance the contrast of the white. Looking at the top mask layer in a viewer, though, I see NOTHING for that layer. Is that because that layer is a negative image and will "print" as a solid fill?

Tomg
Expert
Posts: 1773
Joined: 20 Jun 2015, 14:39

Re: Through Hole Pad without Drilled Hole

#4 Post by Tomg » 21 Sep 2021, 15:15

...couldn't figure out how to move it to the bottom copper layer...
In DipTrace version 4.1.3.1 you can right-click on the copper figure and choose "Properties..." in the context menu (or just double-click on it) to bring up the "Shape Properties" dialog window. In the "Shape Properties" dialog window make the desired selection using the "Layer:" drop-list and click on "OK".
...Looking at the top mask layer in a viewer, though, I see NOTHING for that layer...
Only the outlines of mask layer openings are visible in the Design Area (drop a standard through-hole pad onto the PCB and you will be able to see the outline of the mask opening surrounding it). Using 3D Preview will help you see it more clearly.
Tom

SteveW
Posts: 14
Joined: 05 Oct 2019, 18:49

Re: Through Hole Pad without Drilled Hole

#5 Post by SteveW » 23 Sep 2021, 17:48

Thank you for that information, Tom. The inability to size the imported DXF "Pad" is a little odd, but not a big deal as I will only need 3 or 4 of such "pads" and I can easily import all of them into my library. My company logo is another matter. As I believe I said, my goal here, is to slowly convert all my legacy artwork, some of which is still tape on mylar originals. I have always placed my logo onto both the copper side as well as the top silk screen layers. I have done one experiment and the DXF imports OK with proper fill, IF I use Corel 16. Normally I work in 13, because I just like it better, but the DXF it creates does not fill properly, and the letter "O" fills completely rather than leaving the center open. But as I said, Corel 16 seems to do something different in its export. However, the imported image is HUGE. And if I understand correctly, even though DXF is a vector image to start with, Diptrace does not provide a method to access properties of said image and set height or width??? This seems to be something people have been complaining about for almost a decade. I have searched the forum for new info, but cannot find anything current. Am I just missing something (VERY likely!)?

Tomg
Expert
Posts: 1773
Joined: 20 Jun 2015, 14:39

Re: Through Hole Pad without Drilled Hole

#6 Post by Tomg » 23 Sep 2021, 18:23

From what I have read, DXF is an incomplete format that does not transfer "units" information. This apparently stems from disagreements between competing corporations at a time when everyone was supposed to get together and hammer out universal standards for the format. As a result, DXF requires the user to remember the "units" used in the original drawing (inches/mm/etc.) and to make sure the import settings in the receiving program match. It is possible that a mismatch of the "units" between the two programs could be the cause of the huge drawing figure.

p.s. The PCB Layout editor has a tool that allows you to import a picture (*.bmp, *.png) with the option to convert it into the vector format if you so desire. It also has the ability to adjust the size of the imported object. Go to the main menu and select "Objects" > "Place Picture", or use the "Place Picture" icon at the top to access it.
Tom

SteveW
Posts: 14
Joined: 05 Oct 2019, 18:49

Re: Through Hole Pad without Drilled Hole

#7 Post by SteveW » 23 Sep 2021, 19:30

Thanks, Tom,
No, the original in my Corel drawing was 7.5" wide. I anticipated it coming in BIG. What I didn't realize is that I could not "adjust" it after I got it in. I can try bringing in a bitmap version and see how well Diptrace vectorizes it. It just makes no sense to me, if the original is already a razor sharp vector, why the clumsy approach of changing it to bitmap, then importing it and then having the program re-vectorize it. And I'm CERTAIN Diptrace will not do as good a job in that regard as my original artwork done in vector format. But if that is the only way to get an adjustable image, I will give it a try. Would you suggest I provide a very large bitmap to begin with? Common sense tells me that would be the best way to go. So the vectorization is done on a large image and then reduce it to fit? From your experience, does one format of bitmap give better results when converted by DT? Is there a file size limit on the bitmap?

Tomg
Expert
Posts: 1773
Joined: 20 Jun 2015, 14:39

Re: Through Hole Pad without Drilled Hole

#8 Post by Tomg » 23 Sep 2021, 20:31

My only experience using the "Place Picture" tool involves a few minor experiments. You will have to play around with its contrast setting and it definitely will not be as razor sharp as the original vector drawing. Starting with a large bitmap sounds good to me, just to see how ragged the result will be. I have not used CorelDRAW at all so I'm wondering if there is a way to resize the vector drawing in that program before exporting. I'm sorry that I could not be of more help in this matter.
Tom

Post Reply