View all layers individually?

Making PCB Layouts, Manual routing, Auto-routing, Copper pouring, Updating from Schematic, Manufacturing Output
Post Reply
Message
Author
Exality
Posts: 81
Joined: 28 Sep 2017, 14:08
Location: Seattle, WA area
Contact:

View all layers individually?

#1 Post by Exality » 11 Oct 2017, 12:10

I'm a new DipTrace user, and can't find how to examine all PCB layers individually. I would like to see each of the layers shown in the Design Manager Layers tab, individually, just to look for mistakes.

If I un-check all the layers in the Layers tab in All Layers mode and then enable them one-by-one, the mask and paste layers don't show up. Can I enable them somehow?

Do I need to export to Gerber and use a Gerber viewer to do this?
Gerrit

Tomg
Expert
Posts: 1523
Joined: 20 Jun 2015, 14:39

Re: View all layers individually?

#2 Post by Tomg » 11 Oct 2017, 12:28

DipTrace Solder Mask and Paste Mask Characteristics

* All pads receive an automatic solder mask opening of the same shape and size. Automatic solder mask openings are expanded or contracted by the Solder Mask Swell setting in the Export Gerber dialog window. This is a global default setting that can be overidden by a local setting.

* All pads receive an automatic solder paste area of the same shape and size. Automatic solder paste areas are expanded or contracted by the Paste Mask Shrink setting in the Export Gerber dialog window. This is a global default setting that can be overidden by a local setting.

* Copper planes do not receive an automatic solder mask opening.

* Copper planes do not receive an automatic solder paste area.

* A manually-placed filled drawing figure on the Top/Bottom Mask layer in the Design Area will produce a custom solder mask opening. The size of a custom solder mask opening is not affected by the Solder Mask Swell setting in the Export Gerber dialog window.

* A manually-placed filled drawing figure on the Top/Bottom Paste layer in the Design Area will produce a custom solder paste area. The size of a custom solder paste area is not affected by the Paste Mask Shrink setting in the Export Gerber dialog window.


DipTrace Solder Mask and Paste Mask Viewing

* Automatic solder mask openings are not visible in the Design Area.

* Custom solder mask openings are visible in the Design Area.

* All solder mask openings, a combination of both automatic and custom, are visible in 3D Preview and Gerber Preview.

* Custom solder paste is visible in the Design Area.

* Automatic solder paste is not visible in the Design Area.

* Solder paste, both automatic and custom, is not visible in 3D Preview.

* Solder paste, both automatic and custom, is visible in Gerber Preview.
table2.gif
You do not have the required permissions to view the files attached to this post.
Last edited by Tomg on 04 Feb 2019, 10:35, edited 3 times in total.
Tom

Exality
Posts: 81
Joined: 28 Sep 2017, 14:08
Location: Seattle, WA area
Contact:

Re: View all layers individually?

#3 Post by Exality » 11 Oct 2017, 12:39

You're a gold mine, Tom! Thanks a million. The File / Export / Gerber / Preview thing was just what I was looking for. Now if I could only get it in the Design window so the layers would superimpose and I could step easily through them... :-)
Gerrit

User avatar
KevinA
Posts: 468
Joined: 18 Dec 2015, 15:35

Re: View all layers individually?

#4 Post by KevinA » 11 Oct 2017, 12:44

Exality wrote:I'm a new DipTrace user, and can't find how to examine all PCB layers individually. I would like to see each of the layers shown in the Design Manager Layers tab, individually, just to look for mistakes.

If I un-check all the layers in the Layers tab in All Layers mode and then enable them one-by-one, the mask and paste layers don't show up. Can I enable them somehow?

Do I need to export to Gerber and use a Gerber viewer to do this?
Don't bother with a 'Gerber' viewer.
Export Gerber all layers and then Export a N/C Drill file, open new instance of PCB Editor, Import each Gerber, the first import as New and each layer after that as Add, after all layers are imported import the Drill layer. View each layer, scale and print to E size plotter. You can add the drill to each layer as you import but it takes longer, just add the N/C Drill after all layers are imported.

Tomg, the only Gerber Preview I found was;
PCB Layout > Working with files > Import > Gerber
Import Gerber Preview

And while I was typing this Tomg posted!
Imagine my surprise when after searching, installing, learning to use a Gerber Viewing package I stumbled over Gerber Import in DipTrace Help, one of the reasons I converted the chm help file to an Ebook. RTM

Tomg
Expert
Posts: 1523
Joined: 20 Jun 2015, 14:39

Re: View all layers individually?

#5 Post by Tomg » 11 Oct 2017, 13:09

It never occurred to me to do that, Kevin. An excellent solution to the DipTrace mask viewing issue. Two things to watch out for when importing Gerbers into DipTrace...
1) Disable the [] Enable Real-time DRC option before importing or there may be a long wait for all of the DRC checking to finish.
2) Expect DipTrace to import oval mask shapes as ellipses. I reported this bug a while ago, but so far nothing has come of it.
Tom

eosrisko
Posts: 10
Joined: 04 May 2016, 17:16

Re: View all layers individually?

#6 Post by eosrisko » 06 Mar 2018, 16:14

These tips from Tomg and KevinA I found out by myself but still find it a bit impractical not to be able to see the other layers at design time. When I need to see the spacing between Solder Paste / mask of certain pads, vias or components, I have to export Gerber, open another instance of the PCB Layout and import again to be able to use the Place Dimension tool.

Post Reply