Print Page | Close Window

No Option For Pad Round-off In V2021 Edition?

Printed From: PCB Libraries Forum
Category: PCB Footprint Expert
Forum Name: Questions & Answers
Forum Description: issues and technical support
URL: http://www.PCBLibraries.com/forum/forum_posts.asp?TID=2866
Printed Date: 10 May 2021 at 10:01pm


Topic: No Option For Pad Round-off In V2021 Edition?
Posted By: ExplodingWaffle
Subject: No Option For Pad Round-off In V2021 Edition?
Date Posted: 07 Apr 2021 at 4:29am
Hello- just upgraded to the new version of the software. Enjoying custom footprints and FPX libraries in the free version! 

Sort of bummed about 3D STEP being gone- while it certainly made my 3D views look a lot nicer in Kicad, I suppose they aren't needed.

One thing that I do need that seems to have gone missing from the new version is courtyard and pad-roundoff - is it just gone, or am I missing it? 

I layout my boards on a grid so it's a very useful feature for me.




Replies:
Posted By: Tom H
Date Posted: 07 Apr 2021 at 8:01am
The new V2021 Footprint Expert for KiCad now has these new features: 
  • Options (global user preferences) just File Save to your personal .opt file and edit any value
  • Library Editor to save your data
  • Batch Build
  • FP Designer for custom non-standard packages like connectors
Options have min/max decimal place accuracy up to 6 places. 

Library Editor saves your package dimensions, personal polarity markings, custom 3D STEP color, footprint rotation and footprint pad stack dimensions. 

Select the Footprint panel and enter your pad length x width x gap and save to FPX. You have 100% control now of every pad size and snap grid. 

The 3D STEP is no longer free. You need to pay the yearly maintenance of $299 so we can generate the revenue to enhance that feature with top programmers. You need to move up to the Enterprise version of Footprint Expert for $99 for KiCad. There are no banner ads in the Enterprise version. 

Let us know if you need any help in understanding all the new features in V2021. 

Create your personal FPX file. Create your personal Option file. 



-------------
Stay connected - follow us! https://twitter.com/PCBLibraries" rel="nofollow - Twitter - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn


Posted By: SWB01
Date Posted: 07 Apr 2021 at 8:18am
I don't see the roundoff options in 2021 either. Previous versions had roundoff options all over the place, for just about every footprint element, and I used them extensively to snap geometry to my grid as much as possible.


Posted By: Jeff.M
Date Posted: 07 Apr 2021 at 9:46am
"Roundoff" options are now global and located in 'Tools > Options > Console > Design' in the group 'Decimal Place Accuracy'.

'Minimum' is the minimum number of decimal places to apply. For example a value of 4.1 with a minimum DP value of 2 will round and display as 4.10.

'Maximum' is the maximum number of decimal places to apply.  For example a value of 4.123456 with a maximum DP value of 4 will round and display as 4.1234.

Different numeric units (mils, millimeters, etc.) have their own settings.

Grid placement has it's own setting in the footprint window under the icon 'Manage Layer Display' as Space X and Space Y, emanating from the origin.



-------------
Stay connected - follow us! https://twitter.com/PCBLibraries" rel="nofollow - Twitter - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn


Posted By: SWB01
Date Posted: 07 Apr 2021 at 2:25pm
Originally posted by Jeff.M Jeff.M wrote:

"Roundoff" options are now global and located in 'Tools > Options > Console > Design' in the group 'Decimal Place Accuracy'.
That's not the same thing.

I work on an 0.05-mm grid in Altium. To the extent possible/reasonable (subject mainly to the pin pitch), I want all geometry aligned to this grid. In previous versions, I could accomplish this with roundoff values of 0.05 and 0.10 mm, depending on the parameter.

In this version, we can only round to a certain number of digits, and the smallest number of digits we can round to (in millimeters) is 2. This is equivalent to a roundoff value of 0.01 mm. There is no longer any way to specify a roundoff value of 0.05 mm or 0.10 mm.

That's disappointing. I was hoping for increased flexibility and control over roundoff in this version, not less. In a perfect world, the software would initially do all the calculations at full precision and then stretch and contort it according to some heuristics and intelligence to snap all edges, pad centers, and vertices to my preferred roundoff grid.

I'm going to have to keep using the older version until at least the old roundoff behavior is restored.

(I was so distracted by the lacking/poor hi-resolution monitor support during the beta that I never noticed that core functionality had been changed or removed. Now I'm wondering if there's anything else important that I've missed.)

Originally posted by Jeff.M Jeff.M wrote:

Grid placement has it's own setting
We don't mean the grid within Footprint Expert. We mean making footprints compatible with the layout grid we use in our PCB software.


Posted By: ExplodingWaffle
Date Posted: 08 Apr 2021 at 2:55am
Originally posted by SWB01 SWB01 wrote:

Originally posted by Jeff.M Jeff.M wrote:

"Roundoff" options are now global and located in 'Tools > Options > Console > Design' in the group 'Decimal Place Accuracy'.
That's not the same thing.
--snip--
That's disappointing. I was hoping for increased flexibility and control over roundoff in this version, not less.
What SWB said :) roundoff is a nice feature to have routing on a grid. In addition, decimal place is global- just today I had to go to 4 decimal places to make a complicated IC in the FP designer, but I don't think I'd like to use the same settings on say a 1206 or larger part.
Also- today I discovered that setting "Cathode/Anode Pin Names" to Numeric just doesn't do anything, which is 100% a bug.


Posted By: Ian S
Date Posted: 08 Apr 2021 at 4:08am
I agree with SWB01, the new FPX version is unusable without restoring roundoff functionality.

For example, in V2020 I had the Terminals>Through Hole>Pad Size Roundoff set to 0.05 mm. This resulted in pad diameter and, more importantly, the through hole (drill) size rounding to 0.05 mm.

With the new FPX version the through hole (drill) minimum resolution is 0.01 mm which is not a real world practical resolution when (in my experience) PCB fabricators use drill sizes with 0.05 mm resolution.





Posted By: Tom H
Date Posted: 08 Apr 2021 at 10:55am
We are going to add a new feature in the Pad Stack Rules for PTH hole size roundoff. If your holes are rounded to 0.05 and your pad size calculation multiplier is 2.00 your pad size will always be in 0.05 mm increments. 

The new V2021 Footprint Expert uses new technology for minimum and maximum decimal places. 

You can now go to 2 decimal place for minimum or 6 places. Same for Maximum. This is vastly superior to any CAD tool in existence. 

2 decimal places = 0.01 mm rounding. 

If you want your SMD pad to be in 0.05 mm increments, open the "Footprint" panel and select "Use Mfr. Recommended Pattern" and enter any value you want. You have the ability to round Up or Down. 

Here is a sample QFN and the Footprint pad size values that you can round Up or Down to get your desired result. 





-------------
Stay connected - follow us! https://twitter.com/PCBLibraries" rel="nofollow - Twitter - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn


Posted By: Tom H
Date Posted: 08 Apr 2021 at 11:44am
All reported bugs, including the Anode/Cathode numeric pin names are fixed in the V2021.02 release. 

It only takes us 5 - 10 minutes to fix a bug, so please send me all bug issues directly. 



-------------
Stay connected - follow us! https://twitter.com/PCBLibraries" rel="nofollow - Twitter - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn


Posted By: Quist
Date Posted: 09 Apr 2021 at 3:33am
I don't understand this with rounding of pads.
In Options I have set Unis to mm and Minimum and Maximum Decimal Place Accuracy to 2.
If I calculate a footprint the dimensions under "Manufacturer's Dimensions" (strange name if this is the calculated dimensions by Footprint Expert) are presented with 3 decimal places. +- 0.005 mm in pad size can't have any practical meaning when it comes to soldering etc so I would like it to stick with 2 decimal places. For larger pads even 1 decimal place would be good enough and dramatically reduce the number of pads in our library.

With your solution above Tom, we have to manually edit the dimensions of all pads, this can't be the purpose?


Posted By: Tom H
Date Posted: 09 Apr 2021 at 8:36am
The Land Pattern Naming Convention must have 3 places because of the way it was designed and created. 

XX.XX for the values. 2 places to the left of the decimal point and 2 places to the right of the decimal point. 

I guess you didn't understand 2 X 2 Decimal Place Accuracy like you set in the Console Options. 

Was this the problem that wasn't really a problem? 

When you select Decimal Place Accuracy to 2 min and 3 max, it still produces the same footprint name because that is the standard naming convention. 

i.e.: you can't change the naming convention regardless of your Decimal Place Accuracy because the naming convention is a standard XX.XX for now according to IPC-7351. 

Note: all leading zero's "0" are dropped and ending zero's are not.



-------------
Stay connected - follow us! https://twitter.com/PCBLibraries" rel="nofollow - Twitter - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn


Posted By: Quist
Date Posted: 09 Apr 2021 at 11:07am
Ah, no I was not referring to the Naming Convention but rather to the actual pad dimensions presented under Footprint -> Manufacturer's Dimensions.
I got the impression that no matter what decimal accuracy I put in I got three decimal places on the dimensions but now I can't reproduce the behaviour so it was probably user induced...
I see in our fpx library that we have a different number of decimal places on the pads for different components. That might have been whats fooled me.

Can you please comment on the subtitle "Manufacturer's Dimensions". Who is Manufacturer referring to, component manufacturer or PCB manufacturer? I find it a bit confusing.
Wouldn't it be better to call it something like "Pad dimensions" and the checkbox something like "Use custom dimensions" or similar?



Posted By: Tom H
Date Posted: 09 Apr 2021 at 11:42am
The Manufacturer reference is the Component Manufacturer, not the fabrication or assembly shops. 

The current pad stack and footprint naming conventions are intentionally created in 0.01 mm increments because if you added one more place to accommodate 0.001 accuracy, the footprint name would be too long for most CAD tools. 

Right now, the character limit for a footprint name is 40 characters. If you added one more number to each value the footprint name would be 47+ characters. 

Body Length X Width X Height X Lead Width X Length X Thermal Tab Width X Length 

Same with Pad Stack names. 



-------------
Stay connected - follow us! https://twitter.com/PCBLibraries" rel="nofollow - Twitter - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn


Posted By: Quist
Date Posted: 09 Apr 2021 at 12:34pm
I agree, 0.01 mm is good for naming no matter what the physical accuracy is. I even seriously doubt that there is any practical benefit with going below 0.01 accuracy. Normal trace tolerance in an etch proces is probably around 0.05 mm and might be tweaked down to 0.02 mm.

Regarding "Manufacturer's Dimension": If I open a part in Footprint Expert and would like to see the size of the pads calculated by Footprint Expert the only way I know to do it is to go to the "Manufacturers Dimensions" section and look there. However, this is not the manufacturers dimensions but rather the dimensions calculated by Footprint Expert. 

I don't think the naming is intuitive.



Posted By: Tom H
Date Posted: 09 Apr 2021 at 1:20pm
The pad stack naming convention used in Footprint Expert is available for free download on www.pcblibraries.com/downloads

In Footprint Expert you can double click (or single click + RMB > Properties) any pad and the program will open the pad Properties. 



If you select the Pas Stack name, it will open the Pad Stack Manager. 



The values are grayed out for any Calculator footprint because if you edit it, PCB Libraries, Inc. or IPC cannot be responsible for any typos. 

But you can visually see the pad length and width and corner radius too. 

I can look at any pad stack name and tell you the length, width and corner radius. 

You can control the corner radius in Options > Pad Stack Rules > SMD Corner Rounding > Corner Size Limit 

The default is 0.25 but many users change that value to 0.10 or 0.05. 



-------------
Stay connected - follow us! https://twitter.com/PCBLibraries" rel="nofollow - Twitter - http://www.linkedin.com/company/pcb-libraries-inc-/" rel="nofollow - LinkedIn



Print Page | Close Window