Проблемы при создании Drawing

[UraL 0]

Привет всем участникам!

В чем может быть причина?

ProE вылетает на некоторых больших сборках:

- при входе в Drawing

- при создании нескольких видов

- при экспортировании чертежа в DWG

Используется ProE2001490.

Инсталляция не кривая и работает стабильно.

Похоже проблема в модели, но где копать?

[suslad 1]

Может стоит попробовать обновить версию Pro?? Последний билд ProE2001 — 2004090. Вполне возможно это поможет решить проблему.

[UraL 0]

Привет suslad!

Сейчас обновить систему нет возможности. Нет времени на переустановку и переучивание.

К новому году нужно сдать документацию.

На данный момент у нас только 2 конфликтные сборки. Причем одна из них прекрасно работает в ProE 20.

Гораздо серьезней дела обстоят со второй сборкой - она вся выполнена в ProE2001.

Народ начинает паниковать. Сборка и без того большая (около 7 тыс. деталей), и это только 20-25% от того, что должно быть. Рвутся продолжить работу, по старинке, в AutoCAD.

У кого ни будь были проблемы с циклическими ссылками в сборке?

От инвалидных и некомплектных элементов я избавился.

И где можно узнать, что означает код ошибки - RAISING SIGNAL : Signal number : 11?

[CadCam3d 1]

я работаю в 2001280..ни чего не вылетает и работает стабильно...

так что ...знаешь..может попробовать открыть модель в другом билде..сохранить в нем и уже потом открыть в твоем билде...

мне кажется не коректно записался файл..может исправиться?

[DIMA_M 0]

RAISING SIGNAL : Signal number : 11

Такая проблема бывает из-за отсутствия системного шрифта, который испльзуется для названий датумов, если вы там что-то правили.

Попробуйте найти те детали, из-за которых падает.

Также может быть проблема из-за перехода адресуемого пространства за 1.7 GB, но тогда вам скажут: memory error

Особо характерный случай-удаление невидимых линий на чертеже.

[DIMA_M 0]

UraL

Последний билд 2001 - это 2004290

Рекомендую заказать.

Кстати, вы не под INTRALINK?

[UraL 0]

DIMA_M - благодарю за подсказку.

Сборка действительно занимает в памяти примерно 1.76Гб и вылетает в случае, когда удаляю невидимые линии в чертеже, с сообщением memory error.

Что же получается - это предел? Или это можно как-то обойти?

На машине стоит 2Гб оперативной памяти, еще имеется резерв. Виртуальная память вообще не используется.

Упрощять сборку конечно будем, но иногда ее нужно загружать в полном виде.

Что можно сделать, чтобы обойти эту ошибку?

[DIMA_M 0]

Это проблема 32-разрядной операционки.

Насколько возможно, используйте Simplified Representations.

Для чертежей также рекомендую в CONFIG.PRO пробить allow_refs_to_geom_reps_in_drws yes

И пользоваться drawing representations.

Теперь по поводу Windows.

По умолчанию, под адресуемое простанство выделяется 2 GB.

Можно расширить до 3 GB.

Предупреждаю - работает не всегда.

Вот текст с PTC Knowledge Database.

Description

-----------------

Pro/ENGINEER exits when running out of memory on a Windows workstation prior to reaching the 2 GB memory limit for 32 Bit applications.

Background

-----------------

Currently Pro/ENGINEER running on Windows workstations is a "32-bit" process running on a "32-bit" Operating system. The operating system and the compiler used to create the executable cause Pro/ENGINEER to be constrained by the "32-bit limitation".

With respect to Pro/ENGINEER, the "32-bit limitation" refers to the amount of memory that can physically be allocated for a SINGLE process. Memory is allocated to memory addresses, which in the computing world are represented in binary format (one's and zero's). For example, the following two lines could each represent one memory address:

0000 0000 0000 0000 0000 0000 0000 0000 a(32 zero's)

0000 0000 0000 0000 0000 0000 0000 0001 a(31 zero's and one 1)

Each combination of ones and zeros represents a different memory address or pointer. There are approximately 4 Billion combinations or approximately 4 Gigabytes of memory addresses. This value comes from the number of options for each bit and the number of bits available or 2^32 = 4.3 Billion. The 4GB space is evenly divided into two parts, with 2GB dedicated for kernel usage, and 2GB left for application usage.

This limitation is independent of whether the memory is Swap or Ram.

Alternate Technique

-----------------

Due to memory overhead the actual amount of memory that a single 32-bit application running on a 32-bit operating system can access is generally closer to 1.5GB. In general this limitation is a hard limitation on 32-bit platforms. However, for Windows XP Professional (32-bit) there is a PTC-supported Microsoft procedure for enabling larger process memory addressing. For information how to set this up, please refer to TPI 111330 located at:

<noindex>http://www.ptc.com/cs/tpi/111330.htm</noindex>

Resolution

-----------------

This memory limitation has been confirmed with Microsoft.

Description

-----------------

This document describes the PTC-supported Microsoft procedure for enabling larger process memory addressing under Windows XP Professional (32-bit). This procedure outlined in this document for Windows XP Professional (32-bit) can be used with Pro/ENGINEER 2001 Datecode 2001440 and later. This may be important for some very large assemblies and other situations with high memory requirements.

32-bit operating systems are limited to a maximum of 4 gigabytes (GB) of memory addressing. The actual amount of memory that a single 32-bit application running on a 32-bit operating system can access is generally less than 2GB and closer to 1.5GB. The procedure outlined in this document will enable nearly 3GB to be used for a single application.

64-bit operating systems do not have this same memory limitation and therefore may be a more permanent alternative for very large memory requirements. Windows XP 64 bit systems are supported starting with Pro/E Wildfire Datecode 2003450 and later. PTC will not be releasing Pro/ENGINEER 2001 for Windows XP 64-bit. For further details on 64-Bit Architecture Support, please see TPI 110578 located at:

<noindex>http://www.ptc.com/cs/tpi/110578.htm</noindex> or the customer letter regarding future 64-bit support at: <noindex>http://www.ptc.com/partners/hardware/curre...nium_letter.htm</noindex>

Before using this procedure, one should be aware that there are many techniques within Pro/ENGINEER for reducing the memory requirements of large assemblies, such as simplified representations. These techniques can be found within the Pro/ENGINEER Help documentation, within this PTC TS knowledge database, or through PTC Global Services (by contacting your local PTC Sales representative). Using these techniques is usually a preferable approach because they can significantly improve Pro/ENGINEER's performance (that is, reduce the time to regenerate or perform other operations).

Resolution

-----------------

The following describes the Microsoft's recommended procedure for increasing the per-process memory limit to 3 GB.

Before starting, please read the following Microsoft knowledge base article:

<noindex>http://support.microsoft.com/default.aspx?...b;en-us;Q319043</noindex>

*** Please note that improper modification of boot.ini can render the operating system inoperable. PTC assumes no responsibility for corruption of boot.ini by improper use of BOOTCFG or manual editing. Users will do so at their own risk***

1. Modify the boot.ini on the workstation to include the /3GB switch using BOOTCFG

Windows XP has added a tool called BOOTCFG that can be used to edit the boot.ini file (rather than manually editing the boot.ini file as described in step 4). For more information on BOOTCFG, see:

<noindex>http://support.microsoft.com/default.aspx?...b;en-us;Q291980</noindex>

The following technique can be used to add the /3GB switch to the boot.ini file. From a command prompt, enter the following to add the 3GB switch to the end of the first line of the operating system entry in the boot.ini file (requires administrative privileges):

BOOTCFG /Raw "/3GB" /A /ID 1

Where:

/Raw Specifies the OS options for the boot entry. The previous OS options will be modified.

"/3GB" The 3GB switch

/A Specifies that the OS options entered with the /Raw switch will be appended to the existing OS options.

/ID The boot id. It specifies the boot entry id in the OS Load Options section of the boot.ini file to add the OS options to. The boot entry ID number can be obtained from performing the command: BOOTCFG /Query (this displays the contents of the boot.ini file) at the command prompt.

A reboot is required after editing the boot.ini file. Verify after reboot that the /3GB switch has been added to the boot.ini file. The computer's total virtual memory must then be increased to at least 3 GB in order to enable the switch.

2. Install Pro/ENGINEER locally and patch using IMAGECFG

NOTE: This step is no longer required starting with Pro/E Wildfire 2.0.

Perform a local Pro/ENGINEER installation of Release 2001, datecode 2001360 or later. Make sure you create a backup copy of <Pro/ENGINEER_loadpoint>/<machine_type>/obj/xtop.exe before patching so you can restore normal operation should the file become unusable.

Next, patch <Pro/ENGINEER_loadpoint>/<machine_type>/obj/xtop.exe using IMAGECFG.

As of Release 2001, build 2001440 or later of Pro/ENGINEER, IMAGECFG can be found in: <Pro/ENGINEER_loadpoint>/<machine_type>/obj directory. Imagecfg is also available in the Windows 2000 Resource Kit. For example, to modify the target file xtop.exe:

Imagecfg -l xtop.exe

At this point, the process is complete. Pro/ENGINEER should be able to access more than 2GB of memory. To check if the xtop.exe has been configured properly, run the following command:

imagecfg xtop.exe

This should return a line similar to the following:

Image can handle large (>2GB) addresses

NOTE: As of Pro/ENGINEER Wildfire 2.0, there is no need to run the imagecfg command. Wildfire 2.0 will be able to use the large address by default.

3.Removing the /3GB switch

If you wish to undo steps 1 and 2 above, follow this procedure:

Select Start, Control Panel, and double click on the System icon. Select the Advanced tab, and the Settings button in the "Startup and Recovery" section. Select the Edit button from the "System Startup" section. The boot.ini file will launch in an editor. Remove the "/3GB" from the end of the appropriate boot entry line under the [operating systems] section. Save and close the file. Select OK from the "Startup and Recovery" section. Select the Start button, select Run, and enter "msconfig" and select OK. Select the BOOT.INI tab and verify that the change to the boot.ini file was made. Reboot the computer.

Restore your original version of xtop.exe (prior to the IMAGECFG).

[DIMA_M 0]

И еще.

Одна из проблем, которые пользователи любят создавать себе при работе со сборками - это раздувание объема сборки чрезмерным применением Assembly Cut. А ведь этого можно избежать...

Об этой и других проблемах, а также путях решения - еще один материал с PTC Knowledge Database.

INTRODUCTION

Assembly features have many important benefits but may also have

significant long term effects. The primary benefit is to easily capture

design intent. The potential long term effects include both increasing

the amount of virtual memory required by Pro/ENGINEER and decreasing

overall performance. Retrieval and regeneration performance may be

particularly affected. This document explains these potentially negative

implications and makes recommendations for minimizing them.

In this document, "assembly features" refers to subtractive type

features like cuts and holes that remove geometry from component parts

and have a component intersection list. This document does not apply to

other assembly features that do not remove material, such as datum

features or component features.

DOCUMENTATION RESOURCES

To read additional and more detailed information about Subtractive

Assembly Features and Intersected Components, please refer to the

relevant sections of the Assembly documentation in the Pro/E Help Center.

VISIBILITY LEVEL AND "TWIN" INSTANCES

In order to understand the negative effects of assembly features, the

concept of "visibility level" must first be discussed. The visibility

level of an assembly feature refers to the part or assembly where the

feature geometry may be seen. The visibility level may be at the:

1) Part Level, so the feature will be visible in the intersected

part when it is retrieved on its own,

2) Top Level Assembly, so the feature will only be visible when the

assembly it was created in is retrieved and not visible at any

other lower level, and

3) Sub-assembly Level, so the feature is visible in a sub-assembly

and any higher-level assemblies, but not at any lower-level

assemblies or the part. Note: Starting with Pro/E Wildfire 2.0,

this option is only available with the config.pro option

"advanced_intersection" set to "yes".

When creating an assembly feature, Pro/ENGINEER provides an option to

select the desired visibility level. The Top Level is selected by

default. Designers frequently may change this to Part level so the

feature can be viewed on the part when the part is retrieved on its own.

The Sub-assembly level is used less frequently to show the intersection

in the sub-assembly on its own but not at the part level.

Part level visibility can be convenient for creating identical features

that intersect many parts at the same time. For Part level visibility,

Pro/ENGINEER creates the feature as if it were created with the part

active (in the part’s feature list) but with an external reference to the

assembly. Importantly, this method has minimal effects on Pro/ENGINEER

memory usage and performance and is not the focus of this document.

On the other hand, when the top-level assembly or a sub-assembly is the

selected visibility level, Pro/ENGINEER creates instances, or "twins",

of the parts. This is a necessary requirement to be able to show the

parts both with and without the removed geometry in different contexts

but at the same time. For example, the part may need to be shown in the

assembly window with the feature and in its own window without the

feature concurrently. An assembly may also have the same part assembled

multiple times. Some placement locations of this part may require an

assembly feature intersection but not others.

To be able to show a part’s geometry both with and without an assembly

feature, Pro/ENGINEER must keep different versions of the objects in

virtual memory. Multiple assembly features intersecting multiple parts

will cause memory use to increase in order to keep track of all of the

"twin" objects. The creation of these "twins" during retrieval and

regeneration may also degrade performance.

Further, if the same part is intersected from different assembly levels

each with their own features, the number of "twins" increases and is

equal to the number of assembly levels from which this part component

was intersected.

Also, in addition to assembly features, these "twin" instances are

created for flexible components, inheritance features, mechanisms with

multiple copies of sub-assemblies containing connections, and user

defined part simplified reps.

In general, all of these twin instances will affect memory use similar

to the creation of a family table instance.

RECOMMENDATIONS TO IMPROVE PERFORMANCE AND MEMORY USE

Following are some general recommendations for improving performance

when assembly features are desired. These recommendations may not hold

true in every situation. A section titled Additional Details follows

these recommendations to provide more in-depth discussion and clarify

some of the situations when the recommendations may not hold true.

GENERAL RECOMMENDATIONS

1. Create features with assembly intersection level only when demanded

by the assembly process. That is, drilling, grinding, chamfering and

other material removal operations that take place in real assembling.

2. Use alternatives to features with assembly-level intersections when

possible. Alternatives include: (from fastest to slowest performance)

* Fastest: Create assembly feature using part level intersection.

* Create features on the part level and use external references to

the assembly. That is, create features in the part’s feature list

while the part is activated in the assembly window. This is faster

if backup references are used (see number 3 below.)

* Create assembly features with part level intersection with option

"show feature properties in sub-models".

* Create features in part level using top-down design with skeleton

model, Publish Geometry and Copy Geometry features. For example,

create axis in a skeleton where the hole will be placed, create a

Copy Geometry feature in the part copying the axis, and then

create a coaxial hole in the part.

* Create assembly features with assembly level intersection. This

option has the slowest retrieval performance. Regeneration

performance is generally low but depends on the specific case.

3. Avoid having the same part intersected by assembly features from

different levels. Try to create features at one level only. In other

words, avoid having the same part intersected once from a feature at

the top level and again from a feature at the sub-assembly level.

4. When possible, use external reference control and backup forbidden or

out-of-scope references (available with Advanced Assembly Extension).

In some cases, this will improve the performance of regeneration.

5. Avoid using the "Auto Update Intersects" option unless required by

the design. This function may create unnecessary "twin" instances.

For example, the geometry outline of the feature may be slightly

larger than expected and include more models for intersection than

desired. Instead, manually select the objects to be intersected.

PATTERN RECOMMENDATIONS

1. Create a pattern instead of several independent features if

possible. This may reduce the number of assembly intersections. The

geometry of all features will first be calculated, then intersect

each component once. Therefore, each component is only being

intersected once and only creating one "twin" instance.

2. If a pattern creates many features and most do not intersect every

component, then break up the pattern into separate patterns or

features. Otherwise, each intersection of the patterned feature will

be unnecessarily large in memory because the pattern geometry

definition will be too large for each part. That is, some of the

features created by the pattern will be in the part but not

subtracting solid geometry.

3. Avoid using Group Patterns of assembly features. Instead, use

Ref Patterns whenever possible. Group patterns generally have the

worst performance (retrieval and regeneration) of any pattern type.

Group patterns can often be converted to Ref Patterns by ungrouping

the features, patterning the first feature, then ref patterning the

remaining features.

4. Use the Edit, Solidify (Use Quilt) technique to create one cut

intersection instead of several intersections for the pattern. This

generally has even better performance than creating a simple pattern.

This method has three steps. First, create a pattern of solid

protrusions in a skeleton model representing the reverse of the

pattern geometry to be subtracted. Then create Copy Geometry features

in the assembly copying the Solid Surfaces from the skeleton. Third,

use #Edit, #Solidify (#Cut, #Use Quilt in Pro/E 2001 and earlier)

referencing the copied surfaces in order to create the subtracted

geometry.

ADDITIONAL DETAILS

Placing a feature at the part level may result in slower performance if

the feature is in the middle of the part’s feature list and has children.

When the assembly regenerates, this will cause the features in the part

starting with the part-level assembly feature to regenerate causing an

apparent decrease in performance. Sometimes this behavior is desired, but

if not, the way to avoid this is to place all part-level assembly

features at the end of the part’s feature list.

Pro/ENGINEER users should also be aware that operating system

limitations could cause process memory to be exhausted even though a

large amount of RAM or virtual memory may be available. The symptom of

this would be unexpected exits of Pro/ENGINEER. The techniques above may

help alleviate these memory issues. However, there are also other

solutions available. Please refer to TPI 111330 "Increasing The

Per-Process Memory Limit in Windows XP Professional (32-bit) for

Pro/ENGINEER" for additional information.

[UraL 0]

DIMA_M огромное спасибо!!!

Завтра буду разбираться более детально.

У меня стоит WildFire 2.0 M020

Работаем с ProE 2001490

INTRALINK мы пока не используем, нужно разбираться.

[DIMA_M 0]

Рекомендую М060 - гораздо быстрее работает.

И радиусы на полках ставит без установки скрытотй переменой в config.pro

Кстати, для работы с большими сборками в WF2 проставьте в config.pro

fast_highlight yes

Гораздо быстрее подсвечивает выделенные объекты.

Но есть маленький минусик для дизайнеров - при анализе поверхностей они получаются как помазанные розовой краской. Впрочем, несмертельно.

Включать-выключать опцию можно через CONFIG.

[DIMA_M 0]

Имел в веду через MAPKEY.

[SHARit 2 808]

DIMA_M

Искренне радуюсь вашему участию в форуме.

Большая просьба - не копировать "длинные" источники в тему (неудобно читать), а цеплять как архивы текстовых файлов....

Изменено 16 ноября 2004 пользователем SHARit

[DIMA_M 0]

Понял.Учту.

Просто сильно торопился, не сообразил - а поучаствовать было необходимо срочно.

[UraL 0]

DIMA_M - огромное спасибо за исчерпывающую информацию.

Установили Windows XP, пока все работает, но проблема осталась. Совсем скоро и этой памяти не будет хватать (если делать машину с нормальной детализацией).

Прорабатываем переход на Windows XP 64.

Правда есть одно но - Windows XP 64-bit еще в стадии тестирования, а следовательно и ProE тоже. И раньше 2005 релиз мы не увидим.

На другие операционки переходить не хочется.

Если у кого есть опыт работы на Windows XP 64-bit в ProE было бы очень интересно услышать отзывы.

[SVB 188]

UraL

В чем может быть причина?

ProE вылетает на некоторых больших сборках:

- при входе в Drawing

- при создании нескольких видов

- при экспортировании чертежа в DWG

Прошу прощения, что не вовремя спрашиваю, но что за сборки Вы проектируете? В смысле сколько оперативки отъедают?

Дело в том, что я с коллегами работаю также с большими сборками в Drawing'е, но проблем с вылетом не встречаю. Хотя чертежи достаточно насыщены: вплоть до формата A2x13 и видов более 20 штук и весьма насыщенные. Более того: мой коллега выполняет чертежи в формате А2x8 с теми же примерно 15-20 насыщенными сечениями на весьма смешной машине по конфигурации:

P-III-800, i-815, RAM 512 Mb (pc-133!!!), GF2 GTS (двойка!!!). И это "богатство" работает на WinXP. Правда чертеж выводится несколько десятков секунд, зато потом просто летает (при перемещении и масштабировании) как в AutoCAD'е.

Вообще по опыту могу отметить, что с переходом на Pro/EWF2 работа с чертежами весьма ускорилась. Очень намного. Это обсуждалось в мае-июне этого года.

[SAS_17 10]

Вопрос - нужен ассоциативный чертеж на всю сборку или как?

Без упрощенных представлений здесь наверное не обойтись. Чертежные виды можно делать в отдельных документах и собирать их в одном чертеже через Overlay.

[UraL 0]

В идеале хотелось бы иметь виды ассоциативными.

Вылетал ProE и при создании одного вида. И не только в режиме Drawing, но и при регенерации и сохранении модели.

С помощью DIMA_M эта проблема пока решена.

Упрощенные представления создавать придется, хотя с ними больше неудобств, чем пользы.

Некоторые особенности.

Если сборку грузить в представлении:

- Geometry Rep - экономится примерно 16% памяти, в сравнении с Master Rep

- Graphics Rep - примерно 53%

При переходе в Drawing, вдобавок к упрощенным моделям загружаются и их копии Master модели, и ProE вылетает еще раньше, чем без их использования.

Разумеется, нужно подавлять ненужные компоненты. В этом случае будет выигрыш и в сборке и в Drawing.

А вообще упрощенные представления, это отдельная тема. Тем более, что в ProE имеется несколько способов упрощения модели.

Существенно размеры сборки, у нас, можно уменьшить, изменив точность деталей с завышенной точностью, в некоторых случаях на 40% , установив точность по умолчанию или близкую к ней.

PTC для всех моделей настоятельно рекомендует использовать относительную точность 0.0012. И только в крайних случаях увеличивать эту точность.

Переходить на абсолютную точность, они рекомендуют только в модуле мех.обработки, для получения программ ЧПУ. Увеличение точности увеличивает размер модели и время ее регенерации.

Вот только, как можно посмотреть по всей модели, какая точность деталей установлена? Может как-то можно вывести параметр точности в дереве модели?

[mech 1]

Можно попробывать хорошее средство для работы с большими чертежами - Drawing Representations.

[Basnev 1]

Для насыщенных чертежей очень критичен параметр

enable_hlr_hashing yes/no*

если yes, съедает огромную память и может вылететь.