Consistency errors

Thanks for the offer, but the board has long been deleted and a new board is under construction. I did manage to clear the errors I was having but in doing so I came up with 2 questions.

Question 1:

My DRC rules state that the pad diameter must be a min of 8mil.

My part recomendation is a pad diameter of 8mil.

I have built the part according to the manufacturers recomendation.

Yet if you look at the part and the library side by side the rings of the part on the board are larger than the rings of the part in the library.

Which one will be used in the gerber file, the library or the board representation?

Question 2:

My problem has been with Clearence errors between pins of the same part.

The clearence of the pins according to the library is about 9mil, a fact that was confirmed by another member of this site.

The clearence distance listed in the DRC file is 8mil.

If I set this distance to 4mil, the errors go away. Isn't the distance from one point to another the same as the distance from another to the one?

Why does eagle count both as different distances?

Jim McAuley wrote:

 

Thanks for the offer, but the board has long been deleted and a new board is under construction. I did manage to clear the errors I was having but in doing so I came up with 2 questions.

Question 1:

My DRC rules state that the pad diameter must be a min of 8mil.

My part recomendation is a pad diameter of 8mil.

I have built the part according to the manufacturers recomendation.

Yet if you look at the part and the library side by side the rings of the part on the board are larger than the rings of the part in the library.

Which one will be used in the gerber file, the library or the board representation?

 

Question 2:

My problem has been with Clearence errors between pins of the same part.

The clearence of the pins according to the library is about 9mil, a fact that was confirmed by another member of this site.

The clearence distance listed in the DRC file is 8mil.

If I set this distance to 4mil, the errors go away. Isn't the distance from one point to another the same as the distance from another to the one?

Why does eagle count both as different distances?

As has been stated by myself and confirmed by Jorge several times now, look at the Restring setting in the DRC. Jorge gave you a long and detailed explanation of this earlier this afternoon and it explains exactly what you are seeing with the change in pad size between the library and board. This change in pad size is why setting the DRC clearance rules to 4mil fixes the issue. Don't do that, change the resting setting as we've told you many times.

Best Regards,

Rachael

Jim McAuley wrote:

 

Thanks for the offer, but the board has long been deleted and a new board is under construction. I did manage to clear the errors I was having but in doing so I came up with 2 questions.

Question 1:

My DRC rules state that the pad diameter must be a min of 8mil.

My part recomendation is a pad diameter of 8mil.

I have built the part according to the manufacturers recomendation.

Yet if you look at the part and the library side by side the rings of the part on the board are larger than the rings of the part in the library.

Which one will be used in the gerber file, the library or the board representation?

 

Question 2:

My problem has been with Clearence errors between pins of the same part.

The clearence of the pins according to the library is about 9mil, a fact that was confirmed by another member of this site.

The clearence distance listed in the DRC file is 8mil.

If I set this distance to 4mil, the errors go away. Isn't the distance from one point to another the same as the distance from another to the one?

Why does eagle count both as different distances?

As has been stated by myself and confirmed by Jorge several times now, look at the Restring setting in the DRC. Jorge gave you a long and detailed explanation of this earlier this afternoon and it explains exactly what you are seeing with the change in pad size between the library and board. This change in pad size is why setting the DRC clearance rules to 4mil fixes the issue. Don't do that, change the resting setting as we've told you many times.

Best Regards,

Rachael

Pardon me for butting in...

It appears to me that Jim is saying he's set the DRC rules right but

Rachael (and others) are sure he hasn't. The evidence does seem to

support this, so I wonder... has Jim misinterpreted something? Perhaps

something as simple as entering the required diameter where a radius is

needed? Would it be beneficial for him to post his DRC file for review?

On 02/09/16 19:01, rachaelp wrote:

Jim McAuley wrote:

 

Thanks for the offer, but the board has long been deleted and a new board is under construction. I did manage to clear the errors I was having but in doing so I came up with 2 questions.

Question 1:

My DRC rules state that the pad diameter must be a min of 8mil.

My part recomendation is a pad diameter of 8mil.

I have built the part according to the manufacturers recomendation.

Yet if you look at the part and the library side by side the rings of the part on the board are larger than the rings of the part in the library.

Which one will be used in the gerber file, the library or the board representation?

 

Question 2:

My problem has been with Clearence errors between pins of the same part.

The clearence of the pins according to the library is about 9mil, a fact that was confirmed by another member of this site.

The clearence distance listed in the DRC file is 8mil.

If I set this distance to 4mil, the errors go away. Isn't the distance from one point to another the same as the distance from another to the one?

Why does eagle count both as different distances?

As has been stated by myself and confirmed by Jorge several times now, look at the Restring detting in the DRC. Jorge gave you a long and detailed explanation of this earlier this afternoon and it explains exactly what you are seeing with the change in pad size between the library and board. This change in pad size is why setting the DRC clearance rules to 4mil fixes the issue. Don't do that, change the resting setting as we've told you many times.

 

Best Regards,

 

Rachael

 

--

To view any images and attachments in this post, visit:

https://www.element14.com/community/message/205036

 

The DRC file is from Sunstone Circuits and is available to anyone who would like to download it.

Jim McAuley wrote on Fri, 02 September 2016 22:01

The DRC file is from Sunstone Circuits and is available to anyone who

would like to download it.

 

--

To view any images and attachments in this post, visit:

https://www.element14.com/community/message/205040

So you still haven't changed your restring setting then?

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

None of the settings on the restring tab are causing a problem. I will finish building the board until I get 16 clearence errors. Then change the clearence value to 4mil. Since there are 5 pads 9mil apart on both sides of he board, this will mean that all of the errors are due to Eagle wanting 16mil separation between the pads for 8mil of clearence, the board will pass with no errors and I will generate my gerbers error free.

Jim McAuley wrote:

 

None of the settings on the restring tab are causing a problem. I will finish building the board until I get 16 clearence errors. Then change the clearence value to 4mil. Since there are 5 pads 9mil apart on both sides of he board, this will mean that all of the errors are due to Eagle wanting 16mil separation between the pads for 8mil of clearence, the board will pass with no errors and I will generate my gerbers error free.

There should be 9mil of clearance between the pads IF you have created the part exactly per the datasheet and the pads are the same when viewed in the board as in the library. You said that they were not the same in the board and if this is the case then this will be caused by restring. I don't think there is any other reason for the pads physically being different between the board and the library unless the part in the board is not actually the same part as in the library and is maybe referencing another copy of the library part elsewhere.

EAGLE doesn't need 16mil of separation for 8mil of clearance so although dropping the DRC to 4mil will clear your errors I think your reasoning for why it's working is not correct. If you are happy clearing the errors this way rather than a) fixing the real issue or b) just approving the DRC errors then thats fine, go ahead and generate your gerbers and move on as you've spent far too long on this.

On 3/09/2016 10:36 a.m., Jim McAuley wrote:

None of the settings on the restring tab are causing a problem. I will finish building the board until I get 16 clearence errors. Then change the clearence value to 4mil. Since there are 5 pads 9mil apart on both sides of he board, this will mean that all of the errors are due to Eagle wanting 16mil separation between the pads for 8mil of clearence, the board will pass with no errors and I will generate my gerbers error free.

 

--

To view any images and attachments in this post, visit:

https://www.element14.com/community/message/205043

 

Hi Jim

I see you are running two postings currently and I suspect they are

connected.

#1 Consistency Errors

#2 Editing eagle library

I had a look at the two libraries and the datasheet you referred us to

2nd Sept in #2

Referring to the package within each they are similar and fine apart

from one thing. The diameter of the your pads is 0.048" whereas the

datasheet calls out 0.058"

So amend the pads in the libraries to have diameters of  0.058"

The difference between the rest-ring diameter(0.058) and the drill

size(0.042)  = 16mil which results in an 8mil wide rest-ring.

I then reviewed the Sunstone DRU file mentioned in #1.

That reveals that Sunstone require:

(a) 16mil minimum between drill holes (edges of holes)

(b) 6mil minimum between copper

(c) a minimum of 8mil rest-rings.

You have 0.042 holes at a pitch of 0.067" so the edge to edge spacing of

the holes is 0.067-0.042 = 25mil so (a) is satisfied

The datasheet stipulates pads of diameter 0.058" which will result in an

inter pad clearance of  0.067-0.058 = 9mil so the clearance of at least

6mil is satisfied.

8mil rest-rings can be achieved with your part as we saw earlier so (c)

should be satisfied.

So then on a new board, with the Sunstone DRU file loaded, I added your

part.

Immediately you can sense the inter-pad clearance is not as in the

library. The pads have grown, on the board, driven by the DRC settings.

No black magic here. The DRC is doing exactly what you have told it to do.

As explained in  the other responses, the DRC has calculated the

rest-ring size as 25% of the drill size which results in a rest-ring

width greater than the 8mil minimum set in the DRC and the specific

width we desire if we follow the datasheet faithfully.

But.. we don't have very much space to play with. The rest-ring width

can only grow 1.5mil before the other requirements are not met. Remember

above we have a 9mil clearance and require at least 6mil so we only have

3mil to play with and half of that is added to adjacent rest-rings so

that's 1.5mil each.

So what to do?

I would reduce that 25% of drill size to a lower amount such that the

calculated rest-ring is smaller

Set at 20% (of 0.042) the rest-ring width becomes 8.4mil

The inter pad gap, now 8.2mil, still exceeds the required minimum copper

clearance of 6mil

The DRC check will pass for this component now and the result is very

close to the datasheet.

The rest-rings of other parts will now also be smaller so you need to

review if the reduction suits all parts.

If you have not noticed, Sunstone drills to achieve a finished (plated)

hole size

http://www.sunstone.com/pcb-products/pcbexpress-quickturn/file-drill-summary

The data sheet also calls out a finished hole size.

So a range of drill sizes will result in a single delivered hole size

from the Sunstone hole size range.

On the other hand, the Eagle DRC is calculating using your specific

drill size so on occasions you may be able to manipulate the drill size

in Eagle to satisfy the DRC and yet still get the desired finished hole

size in the delivered board.

I hope this novel has been useful.

All the best

Warren

Hi Warren,

that's a great explanation. You've found the parameter we need

to change. (Set percent of rest-ring smaller)

Freundliche Grüße / Kind regards

Friedrich

-

... benutzen Sie nntp://news.cadsoft.de und einen

funktionierenden News-Reader wie Thunderbird!

... use NNTP://news.cadsoft.de and a

functional news reader like Thunderbird!

Friedrich Bleikamp wrote on Sat, 03 September 2016 05:46

that's a great explanation. You've found the parameter we need to

change. (Set percent of rest-ring smaller)

This really should be no revelation.  The restring settings were pointed to

as a likely source of the problem by several people over several posts.  It

seems it was first mentioned by Racheal two days ago, and was the obvious

culprit once the symptoms were explained.

It always amazes me how someone can come here with a problem, get good

advice, then flail around doing everything except following that advice.

In this case we even had someone delete a month's worth of work (so they

claim) on a board to avoid spending a few minutes actually understanding

the answers he got here, then a few more minutes applying the fixes!

People can do stupid things on their own time as they wish, but it becomes

rude when they abuse volunteer time of those trying to help them in the

process.  Engineering isn't for everyone as it requires logical thinking

and leaving your emotions at home.  Unfortunately we don't have the

technology for software to check this and refuse to work for those not

suited to the process.  Nonsense like this thread will be with us for the

forseeable future.  All we can do is learn from this and cut people off

when they aren't cooperating or doing stupid things.  The signs were there

early in this thread, but were ignored by too many.  Let this be a lesson

that not everyone is worth helping.

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

Am 03.09.2016 um 13:17 schrieb Olin Lathrop:

Friedrich Bleikamp wrote on Sat, 03 September 2016 05:46

that's a great explanation. You've found the parameter we need to

change. (Set percent of rest-ring smaller)

 

This really should be no revelation.  The restring settings were pointed to

as a likely source of the problem by several people over several posts.  It

seems it was first mentioned by Racheal two days ago, and was the obvious

culprit once the symptoms were explained.

 

It always amazes me how someone can come here with a problem, get good

advice, then flail around doing everything except following that advice.

I call that "learning  resistance".

In this case we even had someone delete a month's worth of work (so they

claim) on a board to avoid spending a few minutes actually understanding

the answers he got here, then a few more minutes applying the fixes!

 

People can do stupid things on their own time as they wish, but it becomes

rude when they abuse volunteer time of those trying to help them in the

process.  Engineering isn't for everyone as it requires logical thinking

and leaving your emotions at home.  Unfortunately we don't have the

technology for software to check this and refuse to work for those not

suited to the process.  Nonsense like this thread will be with us for the

forseeable future.  All we can do is learn from this and cut people off

when they aren't cooperating or doing stupid things.  The signs were there

early in this thread, but were ignored by too many.  Let this be a lesson

that not everyone is worth helping.

 

So far I agree with you. [And  I wonder about you that you hold back

that long time without a comment ]

I also feel being lied to by some answers i.e. saying it is a commercial

project. IMHO there can't be no more help then that offered by Morton

Leikvoll.

--

Mit freundlichen Grüßen / With best regards

Joern Paschedag

Am 04.09.2016 um 08:13 schrieb Joern Paschedag:

Am 03.09.2016 um 13:17 schrieb Olin Lathrop:

Friedrich Bleikamp wrote on Sat, 03 September 2016 05:46

that's a great explanation. You've found the parameter we need to

change. (Set percent of rest-ring smaller)

 

This really should be no revelation.  The restring settings were pointed to

as a likely source of the problem by several people over several posts.  It

seems it was first mentioned by Racheal two days ago, and was the obvious

culprit once the symptoms were explained.

 

It always amazes me how someone can come here with a problem, get good

advice, then flail around doing everything except following that advice.

 

I call that "learning  resistance".

 

In this case we even had someone delete a month's worth of work (so they

claim) on a board to avoid spending a few minutes actually understanding

the answers he got here, then a few more minutes applying the fixes!

 

People can do stupid things on their own time as they wish, but it becomes

rude when they abuse volunteer time of those trying to help them in the

process.  Engineering isn't for everyone as it requires logical thinking

and leaving your emotions at home.  Unfortunately we don't have the

technology for software to check this and refuse to work for those not

suited to the process.  Nonsense like this thread will be with us for the

forseeable future.  All we can do is learn from this and cut people off

when they aren't cooperating or doing stupid things.  The signs were there

early in this thread, but were ignored by too many.  Let this be a lesson

that not everyone is worth helping.

 

 

So far I agree with you. [And  I wonder about you that you hold back

that long time without a comment ]

I also feel being lied to by some answers i.e. saying it is a commercial

project. IMHO there can't be no more help then that offered by Morton

Leikvoll.

 

I full agree with Olin and Joern. Unfortunately, my English is

not good enough for me to take part in lengthy discussions.

I always read in the background.

Freundliche Grüße / Kind regards

Friedrich

-

... benutzen Sie nntp://news.cadsoft.de und einen

funktionierenden News-Reader wie Thunderbird!

... use NNTP://news.cadsoft.de and a

functional news reader like Thunderbird!