DipTrace 3.1 beta

[Eternauta]

Novarm has just released the 3.1 beta, new feature:

- Length matching rules.
- Real-time Length Comparison table.
- Layer Stackup table.
- Using Layer Stackup and Pad Signal Delay for trace length and differential pair phase calculation.
- Align objects.
- Switching measurement units with a shortcut in any dialog window (Shift+U by default).
- Hotkeys for selecting sheets in Schematic and for the Measure tool in Pattern Editor.
- Moving all selected trace segments simultaneously (bus editing).
- Permanent Net Highlight option.
- Altium ASCII Import (Schematic, PCB, libraries).
- Eagle XML Import (Schematic, PCB, libraries).
- 11100 new components and 345 new patterns.
- 1120 new 3D models.

[DerekG]

Switching measurement units with a shortcut in any dialog window (Shift+U by default)

Many us have been asking for this for several years .............. so it's great it is now implemented.

Altium ASCII Import (Schematic, PCB, libraries).

Another great feature for me as I'm slowly moving over some of my legacy designs from Altium to DipTrace as updates to the circuits are required.

[sleemanj]

Awesome that they have implemented unit switching.

I can't say I've been especially enamoured with the idea of having massive built in component libraries and having the 3d models distributed like they do though.

I see they have planned "automatic update of libraries and 3D models, this feature is already done, but should be polished and integrated into our web-site", hopefully they do that right.

They really need to take the idea from the tool I wrote for searching the diptrace 3d models at least and make something similar in DipTrace itself, or on their site, preferably for components/patterns too.

[NivagSwerdna]

It would be nice to have some more stock components... my last PCBs have a few very annoying errors where I got the custom components slightly wrong. 

[DerekG]

It would be nice to have some more stock components.

Yes, DipTrace's library operation is the weakest part of their software, mainly because many aspects of their library operation are not so logical.

I understand why the standard DipTrace Libraries are "locked" (can't be changed by the end user) & that we have to generate a new library to save all our own specific parts .............. but this operational requirement is not that easy for new-comers to understand.

I actually preferred how Protel (the predecessor to Altium) did it many years ago. You could design your own component (schematic & footprint) within your actual design space, then highlight it & save it directly to your own library. It was very straight forward & easy to understand. If there was a component in an existing library that was close to what you required, you simply placed it in your current design space, modified it & saved it with a different name.

Do remember, if you are looking for lots of stock footprints, open the standard DipTrace "Pattern" library. That library contains about 95% of all the different footprint variations for SOJ, SOP, SOT, TO devices. etc etc. To modify them, save the specific footprint to your own private library & work on it from there.

[timb]

It would be nice to have some more stock components.

I actually preferred how Protel (the predecessor to Altium) did it many years ago. You could design your own component (schematic & footprint) within your actual design space, then highlight it & save it directly to your own library. It was very straight forward & easy to understand. If there was a component in an existing library that was close to what you required, you simply placed it in your current design space, modified it & saved it with a different name.

You can do this in DipTrace! While doing a PCB layout, you can create pads, silkscreen, mask, etc. right on the board, then select all the items, right click and select "Group into Pattern", now double click the new pattern, give it a name and click OK, then right click the new pattern and select "Save to Library" and it will be saved into the currently select library.

You can also place an existing pattern from the library, right click it and select "Ungroup Pattern", edit it, regroup the pattern and save it back to the library.

Another tip, when doing schematic capture, say you want to create a new transistor: Simply grab the "NPN" or "PNP" component from the "Symbols" library and place it on your schematic, double click and edit the properties (for example, change the name to MMBT3906) now click attach pattern and select SOT-23, make sure the pins are connected correctly (click a pad on the pattern and then click a corresponding pin on the component in the double pane window at the top), now click OK and OK, right click the new transistor on the schematic and save it to your component library. You've just created a custom component without ever opening the Component Editor!

Another nice feature added with DipTrace 3.0 is project specific libraries. Now, you can create component or pattern libraries that are *only* referenced from the particular schematic or layout you're working on. This is nice for those times you need special parts that are only relevant to one particular project and you don't want them cluttering up the main library. For example, you might want some slightly tweaked SMD cap footprints due to manufacturing reasons. Sometimes I'll create patterns that contain just silkscreen with the product logo or something, obviously I don't want that in my main library. Stuff like that.

Honestly, I think Diptrace's library system is very logical and I like it a lot.

The only thing I desperately need is Net Ties. People have been asking for them for years, but it's like they can't grasp the need to tie different nets together, it's infuriating!

[DerekG]

You can do this in DipTrace! While doing a PCB layout, you can create pads, silkscreen, mask, etc. right on the board, then select all the items, right click and select "Group into Pattern", now double click the new pattern, give it a name and click OK, then right click the new pattern and select "Save to Library" and it will be saved into the currently select library.

Thanks heaps Tim.

I learn something new everyday & this will be a real time saver for me.

The only thing I desperately need is Net Ties. People have been asking for them for years, but it's like they can't grasp the need to tie different nets together, it's infuriating!

Can you elaborate further on this please Tim?

I have a quick question. I have added some long dual row headers to my board layout. They are used as "fingerling heatsinks" for some SMD mosfets on the board. I have been lazy & not added them to the schematic as they are just manually layed on top of a copper plane. Is there any way I can "Renew layout from schematic" without having these "fingerling heatsinks" automatically removed or reported as an error?

[timb]

You can do this in DipTrace! While doing a PCB layout, you can create pads, silkscreen, mask, etc. right on the board, then select all the items, right click and select "Group into Pattern", now double click the new pattern, give it a name and click OK, then right click the new pattern and select "Save to Library" and it will be saved into the currently select library.

Can you elaborate further on this please Tim?

I have a quick question. I have added some long dual row headers to my board layout. They are used as "fingerling heatsinks" for some SMD mosfets on the board. I have been lazy & not added them to the schematic as they are just manually layed on top of a copper plane. Is there any way I can "Renew layout from schematic" without having these "fingerling heatsinks" automatically removed or reported as an error?

Okay, so Net Ties: Let's say I have a board and I want an analog ground (VSSA) and a digital ground (VSSD). I want to keep my grounds separate so digital switching noise doesn't creep into the sensitive analog plane. Now, I want these two separate ground planes to connect together at one point on the board, which forms a new net called GND. In software like Altium there is a "Net Tie" component that has three pins (or two, depending) that allows you to tie these separately named nets together.

Now, when you translate this to the layout, you'd have separate copper pour for all three nets; the VSSD and VSSA pours wouldn't connect to each other, but they would connect to the GND pour.

Right now in DipTrace, Novarm's answer is to "use a SMD resistor or create a new pattern with two copper pads touching to tie nets together". However, that doesn't really fly when I need to tie nets together that live on inner layers of a board (since on a 4 layer board GND is usually layer 2 of 4 in the stack) and you can't place patterns on inner layers!

Another example might be this: Say I've got an a WiFi module on my board and I need to lay out the antenna. I'd want to have a special copper pour that has a different clearance (say 15mil) around the antenna and RF trace, to maintain the correct impedance. Now this "RF_GND" pour should electrically be connected to the normal "VSSD" copper pour at the edges, as they should be treated as the same logical net. I'd use a two way net tie on the schematic to infer this.

Does that make sense?

As for your other question, here's what I do:

Create a new component in your library called "Assembly" and just have the symbol be a box with a single pin, don't attach a pattern.

Now, place this on your schematic, double click it, click attach pattern, select your "fingerling heatsinks" and in the double pane window at the top, click the pin of the component and then a pad on your pattern; repeat this for all the pads on said pattern (if there's more than one) so the single pin represents all pads.

Basically the "Assembly" component is a sort of universal component that I can use for one offs when quickly doing a schematic. I generally use it when I want to specify a heat sink or LCD with flat flex cable (since the FFC connector is actually what is on the schematic representing the LCD's connections, I still want the LCD itself to be on the BOM and perhaps have a silkscreen outline for it).

Hopefully that made sense.

[NivagSwerdna]

It would be nice to have some more stock components.

I actually preferred how Protel (the predecessor to Altium) did it many years ago. You could design your own component (schematic & footprint) within your actual design space, then highlight it & save it directly to your own library. It was very straight forward & easy to understand. If there was a component in an existing library that was close to what you required, you simply placed it in your current design space, modified it & saved it with a different name.

You can do this in DipTrace! While doing a PCB layout, you can create pads, silkscreen, mask, etc. right on the board, then select all the items, right click and select "Group into Pattern", now double click the new pattern, give it a name and click OK, then right click the new pattern and select "Save to Library" and it will be saved into the currently select library.nfuriating!

My problem is I create the wrong patterns.     e.g. I recently added a XTAL and though the pads were the front two not on the diagonal. 

[DerekG]

Basically the "Assembly" component is a sort of universal component that I can use for one offs when quickly doing a schematic.

Thanks heaps for this Tim. Much appreciated.

Have you or anyone else used the 3.1 beta? If so, can you confirm that it appears to work well? Any bugs to watch out for?

[djacobow]

You can do this in DipTrace! While doing a PCB layout, you can create pads, silkscreen, mask, etc. right on the board, then select all the items, right click and select "Group into Pattern", now double click the new pattern, give it a name and click OK, then right click the new pattern and select "Save to Library" and it will be saved into the currently select library.

You can also place an existing pattern from the library, right click it and select "Ungroup Pattern", edit it, regroup the pattern and save it back to the library.

Another tip, when doing schematic capture, say you want to create a new transistor: Simply grab the "NPN" or "PNP" component from the "Symbols" library and place it on your schematic, double click and edit the properties (for example, change the name to MMBT3906) now click attach pattern and select SOT-23, make sure the pins are connected correctly (click a pad on the pattern and then click a corresponding pin on the component in the double pane window at the top), now click OK and OK, right click the new transistor on the schematic and save it to your component library. You've just created a custom component without ever opening the Component Editor!

Wow, this is great! I wish I knew this before this past weekend!

[timb]

Basically the "Assembly" component is a sort of universal component that I can use for one offs when quickly doing a schematic.

Thanks heaps for this Tim. Much appreciated.

Have you or anyone else used the 3.1 beta? If so, can you confirm that it appears to work well? Any bugs to watch out for?

No worries, glad to be of help! If you or anyone else has any other questions, let me know. I've become pretty proficient in DipTrace over the last few years. It's good software once you figure out all the little time saving tricks like this. Besides creating new patterns right from the layout, my other favorite trick is setting the Y grid to a separate spacing from the X grid (this can be done from the View menu). This makes creating oddball footprints a breeze!

I have installed 3.1 but haven't had a chance to try it yet. I'll be giving it a whirl tonight and will report back. One thing to watch out for: You can open all your libraries from 3.0 just fine, but if you edit said library and save it with 3.1 it will no longer open with 3.0. So, make a backup of all your libraries before proceeding!

(I run DipTrace in a Windows 7 VM on my Mac, so I keep the DipTrace user folder on my Mac and setup as a shared folder. I have it setup as a local Git repository, letting me roll back libraries and schematics/layouts if there's a problem. The folder is also backed up every couple of hours to my Time Capsule. I've got nearly a thousand custom patterns and components I've created over the years that I wouldn't want to lose, plus 3D models for *everything*, some of which I've had to make myself.)

[DerekG]

I have installed 3.1 but haven't had a chance to try it yet. I'll be giving it a whirl tonight and will report back.

Hi Tim. No hurry, but certainly interested to see how you find the new ver 3.1

I'm working on a couple of boards at the moment ............. & don't want anything broken until they are finished.