Bottom Sil Screen Text Mirrored on JLCPCB

[bostonman]

I'm using PCAD 2006 and created a two-layer (top and bottom) board. It has about four components on the bottom and separate text (revision, date, etc...).

After uploading the gerber files to JLCPCB, it showed the components on the bottom and their reference designators correct (in PCAD 2006, I press 'F' to flip the component to the bottom, and it changes the ref des text to mirrored so I see it as a mirror image - I don't believe a way exists to view it as looking from the bottom).

I also "flipped" the text on the bottom layer for revision, date, etc... thinking that if the component ref designators showed as mirrored in PCAD, then the text needs to show as mirrored too.

This caused JLCPCB to show the bottom layer with the component ref des correct, but the text was mirrored. I went into PCAD and "flipped" it again. Now I can read it normal in PCAD, however, it still showed as mirrored on JLCPCB.

Does anyone know what I need to do so the text isn't mirrored?

[Smokey]

open the gerbers in a gerber viewer like kicad.  check them there before sending them to fab.

PCAD bottom layer silk should look "backwards" in pcad for it to be correct on a bottom layer.

[bostonman]

Thanks!

I was just about to provide an update before reading your reply. Seems I needed to select 'mirror' in the gerber (bottom silk) section.

I saw this before, but feared it would mirror the ref des too, so I didn't select it.

[bostonman]

The PCBs should be arriving mid week.

From the online viewer on JLCPCB, it looked like no matter if I left the text normal or flipped it in PCAD, it showed as mirrored.

I'm just curious, why did flipping it still cause it to be mirrored, and why did selecting 'mirror' in PCAD did the ref des not change? They are on the same bottom silk layer, so I'm not sure why it chose to invert one but not the other.

[bostonman]

Think I spoke too soon about the whole mirror thing.

I swear at one point I "flipped" the text, uploaded it to JLCPCB, and it still showed as mirrored in the gerber viewer. At that point I selected 'mirror' in PCAD 2006 gerbers, didn't "flip" it in PCAD (i.e. it read normal when viewing it), and it showed as normal in the JLCPCB gerber viewer. At that point I kept the text as reading left to right and selected 'mirror' in the gerber options.

Upon receiving the boards today, I noticed all the silk screen was printed normal, but on opposite sites of the board. Also, ironically, I didn't check 'RefDes' on bottom silk screen, so I didn't get any ref des (but I only have three components on the bottom side).

Today I tested things by deselecting 'mirror' in the PCAD gerber options and "flipped" the text. On the JLCPCB gerber viewer, it seemed to appear normal this time. Doubt I'll place another order just because of some misplaced silk screen.

I still lack confidence in the gerber options. Typically I go with the default stuff from my old job (they were tossing PCAD and gave a legal copy to me) in some preliminary designs from them, however, I find discrepancies between boards as for which layers/options were selected.

In one case they had bottom assembly 'mirrored', in another design there wasn't a bottom assembly, etc... The few boards I've had built at board houses usually come out correct, but my layers are basic compared to the elaborate layers in the sample files I reference.

This is the only time a PCB arrived with silk screen in locations I didn't place in that location (although I should have studied the gerber viewer better before placing my order and would have realized the silk screen was opposite).

For future reference, can someone help explain the meaning of the options in the attached (it's a screen shot of PCAD gerber options).

Some is a bit obvious, but what are the differences in all the "top" layers (assembly, silk, paste, mask, and top)? Obviously the bottom will mimic the top, so explaining the top will suffice. Also, what is the meaning of the check boxes on the right?

Silk screen is self explanatory, so that may not need to be explained, but I don't understand things like pads and vias check boxes for all the different layers.

[Kean]

I don't have any experience with PCAD.  I have many years of experience with Eagle and Protel/Altium, and a little KiCAD/others.

In general you should not be enabling the Mirror option for any Gerber/drill files being sent for fabrication.  All the files should be as if you are looking down and through the PCB, so text on the bottom layer will be backwards unless you flip the board in the viewer.

The few times that I would be enabling Mirror option is for PCB prints or assembly drawings of the bottom layers that I will view/print for my own use, so they match the true view from the bottom of the PCB.

The other options on that screen shot I can only guess at.  All the at Layers are what you might think, with Assy being an assembly drawing.  Board is probably the outline.  Not sure about Type.
Then the checkboxes select what to include in that layer.  So a copper or mask layer would include pads.  Copper would have vias.  Drill would have holes.  RefDes,/Type/Value are options typically used only on the Silk layers.  Mirror is as I described above.  Titles would likely add text title to the output, which could be helpful on an assembly drawing, but is unlikely to be needed/useful on the gerber layers as it will just be something that JLC need to remove.

[Smokey]

"Flip" in the text box just reverses the text.  You want to do this for a bottom layer.
Don't mirror anything in the gerbers menu you posted. 

The gerber viewer after you have generated them is the final word.  that is how the boards will be made.  so if you dont' like your gerber viewer output, then you won't like your boards.

[bostonman]

The few times that I would be enabling Mirror option is for PCB prints or assembly drawings of the bottom layers that I will view/print for my own use, so they match the true view from the bottom of the PCB.

I'm unfamiliar with producing drawings for anything other than a board house to produce a board for me, so this could be why all the options and stuff confuse me. As mentioned, I have a few sample boards, but none of them have the same gerbers.

The option of 'mirror' in gerbers makes more sense now too. Due to seeing the text backwards in the gerber viewer made me think 'mirror' was needed. What really confused me is that I accidentally put text on the backside that should have been on the left but on the right side and text that should have been on the right on the left. When I got the "mirrored" PCBs yesterday, I was totally confused because due to mirroring, the text was in the correct locations since it flipped both text on opposite sides.

"Flip" in the text box just reverses the text.  You want to do this for a bottom layer.

I'm uncertain if you're familiar with PCAD, but pressing 'F' flips the part to the bottom which apparently does the same for text boxes (also, non-related, pressing 'L' while routing changes the layer so the trace starts routing on another layer).

[Kean]

The few times that I would be enabling Mirror option is for PCB prints or assembly drawings of the bottom layers that I will view/print for my own use, so they match the true view from the bottom of the PCB.

I'm unfamiliar with producing drawings for anything other than a board house to produce a board for me, so this could be why all the options and stuff confuse me.

Assembly drawings are just that, drawings used during PCB assembly.  They are not needed for PCB fabrication, only for PCBA.  They show the PCB without copper traces, but with the outline of components and their designators (maybe values as well).  Sometimes you need to hide the designators on a silkscreen due to lack of space, so the assembly drawing helps here during manual assembly or future repair work.  Of course, when you are using SMT and have access to a PnP (or use something like JLC assembly services) then the centroid data file for placement is much more useful than the assembly drawings.

[bostonman]

Along with a  licensed version of PCAD, I also inherited their parts library. Unfortunately, much to your feedback, they have unique layers that I don't quite understand; most likely for production purposes.

If I create a part, I need to try duplicating the information on specific layers because I'll get errors when using their PCB template. If I use a black PCB template, then their part libraries give errors. Due to this, I never learned which layers is essential to manufacturing; I only know how to lay out a board and provide gerbers to a board house.

As an example, they have a glue point and a pick point. I assume this would be for a board house to assemble the board on a PNP (I can conduct research on this, I"m just pointing out which stuff I haven't had to worry about).

Also, as mentioned above about unique layers, I never figured out what is so unique that I'm stuck using their blank templates (although it's really not big deal). I've only created five or six boards, and most often the existing part libraries suffice for my needs. Most often I go long periods without needing to create a board, so I find myself annoyed trying to remember all the steps.

In any case, these are reasons for my ignorance on certain aspects regarding PCB layout.