AnsweredAssumed Answered

Many Questions (Former Altium User)

Question asked by melvingalil on Jul 17, 2019
Latest reply on Aug 2, 2019 by melvingalil

Like • Show 0 Likes0
Comment • 24

Hello Folks,

I have many questions:

How do I make all top (or botttom) layer surface mount pads display the color for that layer, regardless of their signal name? (Image 01.jpg)

How do I make all through-hole pads (the annular ring for component pins or vias) display the color for (what Altium calls) "multi-layer"? Grey, perhaps. (Image 01.jpg)

How do I make DRC errors visible at all times (Note how vias are clearly shorting SMT pads here? (Image 01.jpg)

In Altium I can just freely place a via anywhere. At any time. If I placed said free via on a pad or trace, it would assume their net identity of that pad or trace. How can I do that in PADS?

Attachments

Image 01.JPG83.0 KB

No one else has this question

Outcomes

24 Replies

melvingalil Jul 17, 2019 1:23 PM
Mark Correct
Correct Answer
Hello Folks,

How do I make something appear de-selected, when I pretty sure it's not in the current selection set?

Do I have to constantly zoom in and out? 'Cause that seems to work.
Thank you,
Mel
Like • Show 0 Likes0
Actions
chuckt @ melvingalil on Jul 30, 2019 12:48 PM
Mark Correct
Correct Answer
...Not sure what you mean here.
Like • Show 0 Likes0
Actions
melvingalil Jul 17, 2019 1:36 PM
Mark Correct
Correct Answer
Hello Folks,

How do I quickly change the net assigned to a trace, via or free pad?

Thank you,
Mel
Like • Show 0 Likes0
Actions
chuckt @ melvingalil on Jul 30, 2019 1:27 PM
Mark Correct
Correct Answer
You can use the "Add Connection" tool in ECO Mode. If you have two existing nets it will short them together, so you may need to disconnect parts of the net to get the desired outcome. One trick is to route the pin pairs that you want to keep together, leaving unrouted, the pin pairs that you want to split. Then use the delete connection to split the nets.
Like • Show 0 Likes0
Actions
melvingalil Jul 17, 2019 1:49 PM
Mark Correct
Correct Answer
Hello Folks,

How do I change the FREAKING default trace width?

I there a way to partially route traces for a given net? Is the software always going to want to fully route a net, regardless of whether-or-not its creating non-highlighted DRC errors (shorts, etc.)?
Like • Show 0 Likes0
Actions
melvingalil @ melvingalil on Jul 18, 2019 8:27 AM
Mark Correct
Correct Answer
I've tweaked with settings in the Setup> Design Rules, Default (button), Clearance (button) area, opening-up the allowable trace width range.
I've tried changing values in the Tools> Options Text and Lines settings.
I've also tried changing the value in the WIDTH Modeless thing.
None of these things work.
As far as trying to partially route traces I can say that ctrl+left mouse button doesn't work, like, 90% of the time.
Mel
Like • Show 0 Likes0
Actions
chuckt @ melvingalil on Jul 30, 2019 12:53 PM
Mark Correct
Correct Answer
You can open up the range as you say, then use the w modeless commend, but the "default" is set by using the "recommended" setting. You can also use a macro the change the recommended setting if you want. Also, it would be best to use the rules to create net classes that have the trace widths & clearances setup correctly.
Like • Show 0 Likes0
Actions
melvingalil Jul 17, 2019 1:53 PM
Mark Correct
Correct Answer
Hello Folks,

How do I apply a color to a specific net, only when it's un-routed (in rat's nest state)?

How do I apply a different color to different specific net, only when it's un-routed (in rat's nest state)?

Thank you,
Mel
Like • Show 0 Likes0
Actions
chuckt @ melvingalil on Jul 30, 2019 1:12 PM
Mark Correct
Correct Answer
PADS doesn't have a method to have different colors for un-routed vs routed. Its net colors and rats only.
Like • Show 0 Likes0
Actions
melvingalil Jul 17, 2019 4:01 PM
Mark Correct
Correct Answer
Hello Folks,

Can I just place a free random decal from any library into a PCB design?

Mel
Like • Show 0 Likes0
Actions
chuckt @ melvingalil on Jul 30, 2019 1:13 PM
Mark Correct
Correct Answer
Yes, you need to be in ECO mode, then use the "Add Component" tool button.
Like • Show 0 Likes0
Actions
vica_pcb Jul 22, 2019 8:50 AM
Mark Correct
Correct Answer
I'll tell you. I migrated from Altium to PADS too. Yuo'll scream a lot of bad words at the beginning, because PADS follow a different flow and option management rather than Altium. You must understand a very different approach, often way less intuitive than Altium, I have to say. Slowly, things get better but the GUI and some automatism (especially in the layout) remain so much cumbersome (like trace smoothing or even the simplest thing like hilight a net in all schematic).

Said that, before you start doing anything, you should take the Evaluation guide and then do every tutorial included with the sw, including some .pdf like "padslayout_tut.pdf" etc.
You'll find almost every solution in the reference manual (wich is very big and you should use it by searching keywords).
I learned to use it quite well with this approach. It's not fast and is time consuming but is the best way to understand most of the PADS concepts behind the scene.

Unfortunately, there are not many "unofficial" guide like for Altium or Orcad on Internet, because of a silly (IMO) policy of Mentor that has deleted most of them from the net (just search on Youtube, you'll find just trash).
If you want a course, you have to pay for it.

When we are living in a GCC and Open-source era for code, PCB stuff is so reserved... considering that there are such less concepts to understand. Generally speaking, schematics and layout are pretty easy job.

Good luck dude.
Like • Show 0 Likes0
Actions
melvingalil @ vica_pcb on Jul 22, 2019 9:00 AM
Mark Correct
Correct Answer
Thank you, Vica,
I've looked at one of the "eval" things. It is helpful for a quick guide. The online manual is quite large.
I'll have to figure-out a strategy - a road map - for the most effective plan of attack for learning PADS.
First I'll have to figure-out exactly what PADS stuff I have available to me.
(I can't believe there is no proper library manager for any PADS product I have.)
Thank you, dude (or dudette),
Mel
Like • Show 0 Likes0
Actions
vica_pcb Jul 22, 2019 11:24 PM
Mark Correct
Correct Answer
I just want to add one last thing:

don't waste your time with PADS Layout, use PADS Router for as many task as you can. For some operation like plane flooding etc, we are forced to stick with Layout. I use it mostly for components placement too.
But as soon as you have to route, switch to Router. It's more "intelligent" and modern, though users used to Altium will find it very limited too.

PADS Layout it's just a crap, it's like looking in a PC of the '90.
And I think Mentor is the only one in the entire freakin world that need two programs to do what MUST be done in only one.
Schematic side handled by dxd Designer is better. I don't dislike it.

Have fun.
Like • Show 0 Likes0
Actions
chuckt Jul 30, 2019 12:47 PM
Mark Correct
Correct Answer
How do I make all top (or botttom) layer surface mount pads display the color for that layer, regardless of their signal name? - If you have assigned a color to the net in the "View/Nets..." dialog, you won't be able to see the pads in their layer color. The features are mutually exclusive.

How do I make all through-hole pads (the annular ring for component pins or vias) display the color for (what Altium calls) "multi-layer"? Grey, perhaps. - The holes will be displayed in a "complementary" color. You can't make them gray or whatever.

How do I make DRC errors visible at all times (Note how vias are clearly shorting SMT pads here? - You need to run the clearance check if you want see the error markers. It doesn't automatically create/remove them as you create/clear errors. I would recommend setting up a macro that checks the errors with a key stroke... and then clear them with another. I use Alt+1 for Clearance, Alt+2 for Connectivity, Alt+3 for Clear Errors.

In Altium I can just freely place a via anywhere. At any time. If I placed said free via on a pad or trace, it would assume their net identity of that pad or trace. How can I do that in PADS? - In PADS you need to select the net first then RMB/Add Via.
Like • Show 0 Likes0
Actions
melvingalil @ chuckt on Jul 30, 2019 1:02 PM
Mark Correct
Correct Answer
Hello Chuck,

Thank you for the information.

The display comments are helpful. It seems there is something amiss with my computer/PADS compatibility. Vias (and their holes) suddenly disappear at times, only to suddenly reappear. I could be inadvertently hitting the wrong key. I don't know.

The DRC information is helpful, as well.

Regards,
Mel
Like • Show 0 Likes0
Actions
chuckt @ melvingalil on Jul 30, 2019 1:20 PM
Mark Correct
Correct Answer
You probably have the "Display Current Layer Last" setting turned on, and maybe the "Remove Unused Pads" setting also. That combo can make it appear that things are disappearing. like a via that isn't used on layer 3 will not show the capture pad when you switch to L3.
Like • Show 0 Likes0
Actions
melvingalil @ chuckt on Jul 30, 2019 1:24 PM
Mark Correct
Correct Answer
Hello Chuck,

Are you talking about the Options> Global> General> Active layer comes to front setting?

I don't know were he "remove Unused Pads" setting is.

Regards,
Mel
Like • Show 0 Likes0
Actions
chuckt @ melvingalil on Jul 30, 2019 1:30 PM
Mark Correct
Correct Answer
Yes, it's also in a modless commend "D" enter.

The "Remove Unused Pads" is in the Split/Mixed Plane dialog. Options> Routing> Split/Mixed Plane>
Like • Show 0 Likes0
Actions
melvingalil @ chuckt on Jul 30, 2019 2:07 PM
Mark Correct
Correct Answer
Hello Chuck,

It appears I do not have the "Remove Unused Pads" option.

Regards,
Mel
Like • Show 0 Likes0
Actions
melvingalil @ melvingalil on Jul 30, 2019 2:12 PM
Mark Correct
Correct Answer
Hello Chuck,

I want to thank you being a great deal of help.

I do appreciate it.

Mel
Like • Show 0 Likes0
Actions
kbak @ melvingalil on Jul 31, 2019 1:17 AM
Mark Correct
Correct Answer
Hi Mel
If using PADS VX.2.4, the 'Remove unused pads' is in the 'Tools > Options > Copper Planes > Thermals' dialog.

If using PADS VX.2.2, the 'Remove unused pads' is in the 'Tools > Options > Split/Mixed Plane' dialog.

Regards
Klaus
Like • Show 0 Likes0
Actions
johnduquette @ kbak on Aug 2, 2019 6:13 AM
Mark Correct
Correct Answer
"Vias (and their holes) suddenly disappear at times, only to suddenly reappear. " - Do you mean the pads disappear and you only see traces? Hit the <F4> key to toggle your active layer and see if that helps. If your active layer didn't have pads on it (silkscreen, etc.) then Layout won't display the pads on the other layers. After you use <F4> to make a layer with pads active, then you can select your active layer with the layer selection in the upper left corner and put the layer you want on top of the current display.

Clear as mud? I feel your pain, I'm on the Mentor to Altium path right now.
Like • Show 0 Likes0
Actions
melvingalil @ johnduquette on Aug 2, 2019 8:07 AM
Mark Correct
Correct Answer
Hello John,

Yes, that's what I was seeing. I was freaking-out every time it happened, thinking I inadvertently did something to erase all vias.

I actually figured-out the F4 trick by accident just yesterday.

Good luck on your new path. I think you'll be pleased. You'll work faster with a better level of confidence that there's nothing you might have missed. If you integrate PCB's with mechanical things, you'll be please, as well.

Thank you and good luck,
Mel
Like • Show 0 Likes0
Actions

Many Questions (Former Altium User)

Attachments

Outcomes

Related Content

Recommended Content