N/C drill holes not previewing or appearing in .drl file

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

N/C drill holes not previewing or appearing in .drl file

#1 Post by SteveW » 25 Sep 2021, 17:45

I know this is an old problem, but I could not find that anyone had posted a solution. I have a very simple single sided board with non-plated through holes. 24 are of one size and 8 are another size. They are for connectors and arranged in linear arrays. I have double checked every hole in properties to see that it is correct. And I think I have tried every possible setting under the export N/C box. But the generated .drl file is empty except the first few lines defining T1 and T2 tools and their respective sizes. Then there are no position information lines generated. Bringing the zip file into GerbView shows no drill information. Exporting this layer to DXF shows all 32 holes clearly in my CAD system so obviously Diptrace KNOWS they are there, but I cannot find a way to export the .DRL/ Obviously, this is unworkable and I wonder what I am overlooking.

A secondary issue on the same subject. I initially paid Diptrace to do this simple layout for me and worked with Alex. Price was reasonable and I knew as a newbie, I would waste far more time. So when I received the Gerbers and DT file (within a couple days!!), I sent off to JLC PCB for some samples. Boards were fine but were missing a solid mask layer under the top silk, thus reducing the readability. Opening the gerber zip, that layer is truly missing. And one hole size turned out a bit small for the connectors I have chosen. So I decided to make some minor changes. I increased the hole size of the 24 holes without any problems. And I decided to change one part number from vector to true type font. I did not change ANY pattern positions that Alex had used. I DID change the top silk image for one of the connectors to make it easier to identify. Again, no problems..... until I got to the drill file export. After screwing around for about 6 hours trying to figure out what I was doing wrong, I realized I should be able to just use the drill file Alex had created, all the positions were the same. So I edited the file to change the one hole diameter, re-saved and stuck it with the gerber layers to be zipped. Now, when I bring the 7 layers into GerbView for proofing, everything looks fine except the position of the drill hole array does not line up with the pads. And it is off in both X and Y directions by about 0.4". If I use GerbView to open Alex's zipped file, the drill holes appear to be perfect in the center of the pads. I have studied the text of the DRL files and cannot find any line(s) that might introduce this offset. Any idea what might have happened?

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

Re: N/C drill holes not previewing or appearing in .drl file

#2 Post by Tomg » 26 Sep 2021, 10:06

My knowledge on this subject is almost non-existent, but I did some experimenting and found that if both layers are not selected/highlighted then the coordinates will not be exported. As far as things not lining up, you might look to see if the "[x]Use Design Origin" option has something to do with it. If it isn't enabled then the "Offset" settings will come into play.
nc1.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: N/C drill holes not previewing or appearing in .drl file

#3 Post by SteveW » 26 Sep 2021, 10:24

Hi Tom, FWIW, I did use the exact same settings you show above checked. The only thing I note is that under tools on the right, my screen comes up with the two correct drill sizes but no tools. I have tried selecting the Auto button and I have manually entered T01 and T02. But when I try to preview, I either see nothing or sometimes just the one row of 8 holes and the 24 are gone.
As far as the offset goes, it is not material as I am using Alex's file with just the diameters modified in a text editor. And his file lines up properly in Gerbview with his original .GBR files, but not with my new ones I exported from my slightly modified file. And I have checked both designs, his and my modified one. Both outlines and layers appear identical, nestled into the upper right quadrant of the crossed hairs on the screen. Perhaps Alex has something in there that changed the origin by the 0.4 in each direction. But if so, I would think his original would display differently.
I really appreciate all the time you are devoting to my ignorance, although I have used CAD programs and other board layout software with far fewer anomalies than I see with DT. With that said, I still think it is a good choice for my needs, which are really simple compared to most.
Steve

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

Re: N/C drill holes not previewing or appearing in .drl file

#4 Post by Tomg » 26 Sep 2021, 10:46

I know this is probably way off on an unrelated tangent, but just for curiosity's sake go to the main menu in the PCB Layout editor and select "File" > "Layout Information..." to open up the "Design Information" dialog window. Does the "Holes" information listing track with what you believe is on the board? Sorry to be throwing darts in the dark here.
Tom

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

Re: N/C drill holes not previewing or appearing in .drl file

#5 Post by SteveW » 27 Sep 2021, 18:27

Hi Tom, I think you have hit on something.... at least a clue, but I have no idea what I am seeing. Hopefully it will tell you something. I am attaching a screen snip of the Design Information boxes from Alex's file on the left and mine on the right.
So what I am seeing is that both boxes show 32 holes, both show all the holes plated (which is not what I want), but my info shows 24 as blind/buried. ??? I have no idea how that is even done, much less how it happened as I modified Alex's file. And mine only shows 8 through holes. What I want is 32 holes, 2 sizes, all the way through the board, non-plated with pads only on the bottom copper layer. Alex had a pattern he used and I THOUGHT I just retained that. But something must have happened to lose/change the hole information on said pattern. It shows locked as well and I thus cannot select a single pad to look at its properties. I can unlock it, of course. I originally did take his pattern into the pattern editor, re-named it, changed the top silk image and saved it in my own library. Then I brought it back into the drawing in place of the one Alex had used, centered it exactly over the other one, then deleted Alex's. Obviously something I did messed things up. I used manual routing to connect the few pads and did not take any time to establish nets first. I didn't think it was necessary.

1) If I select pads individually (or in groups) and go to pad layers and select just bottom, isn't that all I have to do to ensure there will be no top pads or plating? Or is it just sufficient to tell a board house that ALL holes are non-plated?

2) I'm inclined to start from scratch on that one connector pattern. It is only 24 arrayed holes with my own top silk image. Somehow, these holes converted to blind/buried and maybe that is what is screwing up the drill export.

Any other thoughts?

BTW, I thought maybe I had forgotten to check the Origin box and thus was getting the offset on all my Gerber layers. But when I opened the file back up and went to export and preview each layer, the "use drawing origin" was already checked. But just for grins, I went and re-exported all 6 layers with the box definitely checked. Added Alex's drill file, re-zipped them, and opened in GerbView. VOILA..... all layers aligned. I fought with that for hours. No idea what changed other than closing and opening the program on different days.

On the other subject we were discussing of bringing in a logo: I did some experimenting in CorelDraw. As mentioned, original vector drawing was 7.5 inches wide. And yes, Corel can easily scale it to any size but we discussed keeping it large for sharper edges. I did reduce it to 50% first, making it 3.75" wide and 1" high. I filled it with black, then removed the hairline outline so that it was just a "fill" image with a little less "weight" (thought it might silk screen better with finer lines) . Then converted it to a bitmap in Corel. Used a high DPI of 2400, again for good edge sharpness since my logo is almost entirely straight edge angled shapes. Also chose Black and White as the export type rather than a gray scale - to keep the file size down. Saved as a .png with no background. Imported into my drawing as a vector conversion. I must say I am impressed with DipTrace's bitmap conversion to vector..... And this coming from a decades long Adobe and Corel graphics "expert". At the 1" height, it looks perfectly sharp. Reducing it to 10% to fit properly seems to retain the sharpness. So I think that although a vector import that was scalable would be a dandy feature, the workaround seems to work just fine. Next I need to try and move a logo image from the top silk down to the bottom copper layer. Haven't tried to confuse myself completely with that one yet. I'll probably be back to you with THOSE problems. Sorry!

Steve
You do not have the required permissions to view the files attached to this post.

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

Re: N/C drill holes not previewing or appearing in .drl file

#6 Post by Tomg » 27 Sep 2021, 22:33

...1) If I select pads individually (or in groups) and go to pad layers and select just bottom, isn't that all I have to do to ensure there will be no top pads or plating? Or is it just sufficient to tell a board house that ALL holes are non-plated?...
It seems reasonable to me that if you don't include the Top layer in the Gerber file set and remember to tell them that all holes are non-plated, that could work. Check with them first, though, because not seeing the Top layer included in your Gerber files might upset their apple cart. On second thought, that will probably create problems with the mounting holes, so forget that idea.

Another possible way to get non-plated through-holes sporting pads only on the Bottom side would be to place SMD pads on the Bottom side and overlay them with mounting holes of the desired diameter (make sure their Keepout size = 0). Error flags might appear because of the overlaid holes, but you should be able to ignore those. When routing, the "[ ]Follow Rules" option will have to be disabled. I don't know how your board house will feel about the overlays so you might want to ask them if they can handle it without freaking out. Your Gerber set should be able to include both the Top and Bottom layers.

Keep in mind that the above musings are only the result of some uneducated guesses on my part.
Tom

Alex
Technical Support
Posts: 3593
Joined: 14 Jun 2010, 06:43

Re: N/C drill holes not previewing or appearing in .drl file

#7 Post by Alex » 28 Sep 2021, 06:47

There are pads only in your design. TH pads always have plated holes in DipTrace. So you can export holes to N/C drill file as plated holes, then specify board house that holes are supposed to be non-plated. Rename drill file correspondingly to avoid confusion.

Solder mask layer is negative on its nature. If there are shapes on top mask layer then there will be openings on these areas on real board. At the contrary, if there is nothing on top mask layer then the top side will be fully covered. So you can export empty top mask layer and send to board house. But there is possible problem. They may trigger empty file as an error or ignore it silently. Therefore, it would be better to talk with board house and specify you need solder mask on both layers.

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

Re: N/C drill holes not previewing or appearing in .drl file

#8 Post by SteveW » 04 Oct 2021, 15:13

Just a couple other thoughts and observations. Alex mentioned in a previous post that to make the board single sided, I should use the 'hide ring on layer' option to only display the pads on the bottom copper layer. A couple other people said that upon right clicking a pad, you could go the 'select layers' option and deactivate the top layer. And that was easy so that is what I did. But I find that this action is apparently what causes the holes to then be labeled as blind/buried rather than through hole and then the export to N/C drill fails. I don't know if this is a bug or intentional. But If I just hide the pads as Alex suggested, then the drill file is created properly. Don't think I understand but I don't need to as long as I can make it work that way.

Post Reply