How to Use the SolidWorks Design Checker - Part 4

In part 4 of this series on the SolidWorks Design checker, we will take a look at a way to have SolidWorks learn standard checks from an existing document. It is quite simple actually. SolidWorks Design Checker has a tool called Learn Checks Wizard. This tool is used to retrieve design checks based on attributes from an existing SolidWorks part, assembly, or drawing document. For this blog article, I will keep it very simple so that you get can get a basic concept of what the Learn Checks Wizard does. Let’s get right into an example.

Open a new SolidWorks Part Document. I will use the default part document from the tutorial folder. This is one of the templates that come right out of the box. Let’s see how SolidWorks chose to set up all the options.

Pull down the “Tools” menu and pick Design Checker > Learn Checks Wizard. On the right side of your screen, in the Task Pane, the Design Checker tab appears. Here you can see a list of all the different types of checks that are available. For example, the first one is Document Checks. Let’s expand Document Checks.

Underneath Document Checks is a list of checks related to the document itself. In front of each check is a white box. Click in the white box to select the check. As you select a check, information about that check appears below. So, if you select Dimensioning Standard, you can see that the Dimensioning Standard is set to ISO.

Go ahead and click around to see some of the checks available including: Document’s Arrow Style, Custom Property, Units Setting, Note Font, Dimension Font, Detail Font, Section Font, View Arrow Font, Surface Finish Font, Weld Symbol Font, Table Font, Balloon Font, Detail View Label Font, and Section View Label Font. As you select each check, you will see that whatever the current document is set to will be applied to that value in the check.

Some checks do more than just display the checks available, they actually allow you to input some data. Take for example Dimension Checks. Scroll down to Dimension Checks and expand it. Select Dimension’s Font Check. A red box appears and asks you to select the specific dimensions that have the qualities desired for this check. Notice what happens if I pick a dimension from a simple sketch while in Edit Sketch mode.

The dimension I selected appears in the middle panel and the dimension parameters are captured. It is just that easy to have SolidWorks generate checks from you current document. Once you go through the list of checks and select the ones that you want to be learned, click the green check box in the upper left corner of the Task Pane. The checks are generated and the SolidWorks Design Checker opens, allowing you to save a .swstd file to use as a template to check other SolidWorks part, assembly, or drawing documents.

In conclusion, Learn Checks Wizard is a great WYSIWYG way to create checks with the SolidWorks Design Checker.

We hope this series has given you an insight to how to access the tools in the SolidWorks Design Checker.  Please check back to the CATI Blog as the Dedicated Support Team will continue posting new series of articles every month that go further into the details of many of the SolidWorks tools. All of these articles will be stored in the category of Daily Dose.....of SolidWorks Support and links to each article with their release date are listed below:

• SolidWorks Design Checker - Part1 (Bryan Pawlak 5/7/14)


• SolidWorks Design Checker - Part2 (John Van Engen 5/8/14)


• SolidWorks Design Checker - Part3 (Blake Cokinis 5/12/14)


• SolidWorks Design Checker - Part4 (Neil Bucalo 5/13/14)

Neil Bucalo, CSWP
Certified SolidWorks Support Technician 2013
Computer Aided Technology, Inc.

How to use the SOLIDWORKS Design Checker – Part 2

Checking Against an Existing File

The Check Against Existing File tool validates the active document against checks created from existing files.

Supported file formats are:

• DWG files (*.dwg)


• Part (*.sldprt, *.prt)


• Assembly (*.asm, *.sldasm)


• Drawing (*.drw, *.slddrw)


• Template (*.prtdot, *.asmdot, *.drwdot)


• Drafting Standard (*.sldstd)

Here we have 2 similar documents. They don't have to be identical but these images are for illustration purposes. In these pictures some of the fonts and styles were changed. We will use the first document to be our standard. The second document needs to be checked.

    

Activate the document that we want to check and go to the design checker. Where do we find the tool?

When you run Check Against Existing File, Design Checker creates a new standards file based on the file you selected, opens the file in the Build Checks module, validates the active document, and shows the results in the Task Pane as seen in the following images.

WHOA!! That's a lot of checking!!

You can specify which items are important and which are minor. To see the results of the active comparison return to the drawing being checked and look at the task pane for the results.

Each of the checked items that didn't pass show up in the task pane and can be dealt with on an individual basis or auto corrected all at the same time!

We hope this series has given you an insight to how to access the tools in the SolidWorks Design Checker.  Please check back to the CATI Blog as the Dedicated Support Team will continue posting new series of articles every month that go further into the details of many of the SolidWorks tools. All of these articles will be stored in the category of Daily Dose.....of SolidWorks Support and links to each article with their release date are listed below:

• SolidWorks Design Checker - Part1 (Bryan Pawlak 5/7/14)


• SolidWorks Design Checker - Part2 (John Van Engen 5/8/14)


• SolidWorks Design Checker - Part3 (Blake Cokinis 5/12/14)


• SolidWorks Design Checker - Part4 (Neil Bucalo 5/13/14)

John Van Engen
Senior Technical Analyst
Computer Aided Technology, Inc.

How to use the SOLIDWORKS Design Checker – Part 1

This month we are going to begin a deep dive into the SOLIDWORKS Design Checker. We are going to take a look at how this tool allows a company\user to maintain consistency across their documents. The Design Checker is a utility that verifies settings in a document such as dimension standards, annotation settings, fonts, materials, units, ect.

The SOLIDWORKS Design Checker is an add-in that is available in SOLIDWORKS Premium and SOLIDWORKS Professional only. This can be turn on by going to Tools, Add-ins and checking the box next to SOLIDWORKS Design Checker.

The Utility can be launched from the Tools pulldown menu (with or without a document open)

The Design Checker will open with a dialog box allowing you to select one of the available modules.

The available modules are:

Build Checks – use this tool to set the requirements for evaluation.

Check Active Document – use this tool to validate your current document.

Check Against Existing File – use this tool to validate the active document against design checks from existing files.

Learn Checks Wizard – use this tool to retrieve design checks based on attributes from an existing SOLIDWORKS document.

 

The Welcome to SOLIDWORKS Design Dialog box allows you to access the following options:

Create a New Standards File – build a new .swstd file.

Open an Existing Standards File – browse to a .swstd file to check an active document.

 

Check Active Document

The Check Active Document tool uses the design check standard that was created to check your open document.

Setting the File Location to search for .swstd files

1. Click Tools, Options, System Options, File Locations


2. Select Design Checker Files in the pull down menu


3. Add the path to the folder location that contains the .swstd files.

Running Check Active Document

1. 
   
   Launch the Check Active Document from Tools, Design Checker, Check Active Documents.
   
   

   A Design Checker tab opens in the Task Pane.

   
   


2. 
   
   In the Design Checker task pane:
   
   
   
   
   1. Click the + symbol to add a new standards file
   
   
   2. Click the – symbol to remove a standard from the list
   
   
   3. Check one of the boxes to select an existing standard to run on the active document
   
   
   4. Click Select File to open a document to check.
   
   

1. Click the Check Document to check the active document and display the results based on the selected standard.


2. 
   
   Depending on the passed and filed checks, the following messages are displayed:
   
   
   
   
   1. A message that your document is per standard.
   
   
   2. A list of failed checks organized by criticality level.
   
   

Correcting Filed Checks

To correct failed checks:

1. Expand the individual notes to show the Actual Value and Preferred Value(s)


2. Select Auto Correct All to fix everything automatically, or select one or more failed checks and click Correct Selected to fix the failed checks individually.


3. Click the Refresh button at the top of the window to revalidate the document.


4. Click the red X in the upper right corner to close the tab without saving the changes.

Validating Additional Documents

To validate additional documents:

1. Check the first active document and make corrections.


2. Switch to another open document.


3. Click Check Document to validate the second document using the same settings.


4. Switching between the active documents will allow you to view the various results.

The Design tool is a powerful tool that helps keep consistency in our files. This is just the tip of the iceberg. Please be sure to check back as our tech team continues to uncover and explain the additional functions inside of the SOLIDWORKS Design Checker.

We hope this series has given you an insight to how to access the tools in the SolidWorks Design Checker.  Please check back to the CATI Blog as the Dedicated Support Team will continue posting new series of articles every month that go further into the details of many of the SolidWorks tools. All of these articles will be stored in the category of Daily Dose.....of SolidWorks Support and links to each article with their release date are listed below:

• SolidWorks Design Checker - Part1 (Bryan Pawlak 5/7/14)


• SolidWorks Design Checker - Part2 (John Van Engen 5/8/14)


• SolidWorks Design Checker - Part3 (Blake Cokinis 5/12/14)


• SolidWorks Design Checker - Part4 (Neil Bucalo 5/13/14)

Computer Aided Technology, Inc.

Helical Sheet Metal Modeling

Ever needed to model a helical shaped bent/twisted/rolled sheet metal part in SolidWorks?  Sounds like fun huh?  Actually it is pretty simple with a few little tricks and the Lofted Bends command. 

Start by creating a helix based on a height and revolution.  As I am working with a single part for auger flighting, I am creating my shape for 1 revolution with the intent of add multiple instances in an assembly for final welding.  Second, I will create two perpendicular lines as independent sketches on two perpendicular planes.  Now we can create our Swept Surface using the Helix as a guide curve.

Next, we create an opening for the shaft by creating a sketch to match the ID of the flighting.  We create a Surface Trim command to remove this surface data.

 

Finally we are able to create two 3D Sketches by selecting each edge of the helical swept surface and using Convert Entities for each one.  With these two open profile 3D Sketches we can create a Lofted Sheet Metal feature.  All we need to do is select each one, and chose a thickness to apply.

There you have it a sheet metal lofted part based on a helical swept path!  Enjoy!

Brian Reel
CATI

SolidWorks Filters

SolidWorks Filters: Users often turn on filters without intending to do so, why?

This usually happens when we type new names for features in the Feature Manager Tree.

The SolidWorks' graphics area can become active if you bumped the touch pad or mouse stick on your laptop. The letter "e" is a shortcut (in the graphics area) to filter for edges and this turns on the blue funnel on our cursor. It also makes it impossible to select a model face to start a sketch.

Checkout the following video to see how it works:

 

 

 

 

SOLIDWORKS, Duct Tape and Bailing Wire, Creative solutions to everyday problems

CATI's monthly contribution to the SolidWorks Blog was posted last week and SOLIDWORKS has a monthly 22 minute webinar series and for the month of May they have asked me to bring out some of my Redneck Workarounds.

The presentation is; SOLIDWORKS, Duct Tape and Bailing Wire, Creative solutions to everyday problems

The presentation focuses on is finding creative solutions and different methods of solving modeling and administrative problems. Attendees will learn how day-to-day modeling and administrative challenges are overcome with some inventive and sometimes bizarre methods.  The goal is to inspire SOLIDWORKS users to think more creatively and inventively for solving your every day design issues.

You have two opportunities to view the webinar on May 13th at 11am and 2pm Eastern time, to register please use the links below.

http://www.solidworks.com/webinar_solidworks_duct_tape_11am

http://www.solidworks.com/webinar_solidworks_duct_tape_2pm

To view the article use the link below.

http://blogs.solidworks.com/tech/2014/04/solidworks-duct-tape-and-bailing-wire-creative-solutions-to-everyday-problems.html

Josh Altergott

Support Manager

Computer Aided Technology, Inc.

www.cati.com

SolidWorks Task Scheduler - Part 4

Welcome to part 4 of our blog series covering the SolidWorks Task Scheduler.

In this blog article, we will cover the last four sections: Render and Animation, Convert Workgroup PDM Files, Print Workgroup PDM Files, and Export Workgroup PDM Files

 

Render and Animation

Render and Animation manages rendering and animation tasks. In the SolidWorks Task Scheduler dialog box, if you click on Render and Animation, the Help topic pops up.

The Help file states, “You can use Task Scheduler to manage rendering tasks you set up in PhotoView or animation tasks you set up in Motion Studies. You must start the tasks in PhotoView or Motion Studies before you can manage them in Task Scheduler.” What that is telling us is that all of the options for these tasks are controlled within SolidWorks itself.

Scheduling PhotoView Renderings

PhotoView 360 is a SolidWorks add-in that produces photo-realistic renderings of SolidWorks models. The rendered image incorporates the appearances, lighting, scene, and decals included with the model. PhotoView 360 is available with SolidWorks Professional or SolidWorks Premium. If you do not have this Add-in, then you can skip to the next section.

In SolidWorks, add in PhotoView 360 and then pull down the Photoview 360 menu and pick Schedule Render. (This is also found on Render Tools toolbar).

This option allows you to schedule a rendering at a specified time and save it to a file. This is extremely useful since large renderings require a lot of CPU usage and can take several hours to complete. Rather than babysitting your computer, you can schedule this process at a time when you are not around.

In the Schedule Render dialog box, give the output file a name. Note that the default file type is set in the PhotoView Options PropertyManager, in Image format.

Next, set the directory where the file will be saved.  Note that the default directory is set up in the PhotoView Options PropertyManager, in Default image path.

The Settings button opens a read-only list of settings related to the rendering.

Before you schedule your render, make sure that SolidWorks Task Scheduler is open. SolidWorks Task Scheduler must be open at the time of the render. SolidWorks itself does not have to be open.

You can schedule a Start Time and Start Date that is convenient for you. If Start after Previous Task is checked, then the start time and date will be grayed out. Start after Previous Task is only available when another rendering is scheduled.

Click the Finish button when you are ready to schedule the task.

Scheduling Animation Tasks

From a SolidWorks motion study, click Save Animation  (MotionManager toolbar).

Click Schedule in the Save Animation to File dialog box.

Select options in the Video Compression dialog box and click OK.

The Schedule Animation dialog box is really easy to use. You simply name your task, and specify a file name and location. Setting the start and end time is the same as before. Remember that if Start after Previous Task is checked, then the start time and date will be grayed out. The View Settings button lets you check the animation settings.

Click Finish. That’s it! Switch over to the SolidWorks Task Scheduler. Next to Show Task, select Scheduled to see the tasks you created.

Convert Workgroup PDM Files

Many users and administrators become very stressed when a new major release of SolidWorks comes out. With each update of SolidWorks, the files have to be updated to the newest version. To help alleviate the need for a bottle of your favorite Antacid, the SolidWorks Task Scheduler automates the conversion process for you. Convert Workgroup PDM Files does exactly that. It converts Workgroup PDM Files Vault files that were created at an earlier SolidWorks release to the current release. You must have a Workgroup PDM client license installed on the computer using the SolidWorks Task Scheduler.

Before we get started, please take a note of a few things:

• Back up all files before converting them


• Only vault administrators are allowed to convert files.


• The vault is locked automatically during the conversion process.


• All converted documents are opened in a resolved state (not lightweight). The computer must have enough memory to handle the resolved components.


• You can convert the entire vault or specific projects.


• You can specify that only the latest revision be converted.


• The list of files that convert successfully appears in Task Scheduler.


• Running the task on the vault server is not recommended because of the performance requirements.


• The system you run the task on must meet the recommended memory requirements for SolidWorks. Visit: http://solidworks.com/System_Requirements.

Note that you must be logged into Workgroup PDM first either through SolidWorks or SolidWorks Explorer. With that said, let’s get started. In the SolidWorks Task Scheduler dialog box, click Convert Workgroup PDM Files.

You will be prompted to type in your Workgroup PDM user name, password, and the name of the computer with the Workgroup PDM Vault to login when you click on the Workgroup PDM tasks. The default user name for the administrator is pdmwadmin and the default password is pdmwadmin. You must have administrative privileges to update files. You are prompted for your user name, password, and computer name only the first time you create a Convert Workgroup PDM Files task in the current SolidWorks Task Scheduler session.

First, name your task. The default name is Convert Workgroup PDM Files, but you can use any name that you like. You are then given the option to update the entire vault or to specify projects and file types. We recommend choosing Update by project and files instead of trying to convert the complete vault in one operation.

Next, click the Add Project button. Only projects to which you have read-write access are displayed. Ask your administrator to enable read-write access to the projects you need to update. Select one of your projects from the list that appears in the Workgroup PDM Projects dialog box. You can include documents in subprojects in the print operation as well. You can add as many Projects as you wish. Every time you use the Add Project button, it adds another project to the list. If you add a wrong project or you change your mind, you can use the Delete button to remove a project from the list. To the right of the Project list is the column File Name or Type. You are given the ability to filter the files in a project based on type: parts (*.prt, *.sldprt), assemblies (*.asm, *.sldasm), drawings (*.drw, *.slddrw), all SolidWorks files (*.sldprt, *.sldasm, *.slddrw), or all files (*.*). You can select a type from the list for each project.

Note: If a selected project uses standard library files from a shared location, these files must be accessible to the computer on which you are running the update.

Task Schedule

Whether you need to update your vault files just this one time or on a regular basis, you can schedule this to occur automatically. What if you forget which files you updated and which files are not updated yet? No problem! The Task Scheduler detects files that have already been updated and does nothing at subsequent tasks.

Task Scheduler lets you set the schedule. Pick from Once, Daily, Weekly, or Monthly. You can even control the exact start time and date. Note that Daily means that the task will run every day from the specified date, including Saturday and Sunday. Weekly means that the task will run on the same day of the week, like every Friday, and Monthly occurs on the same day of the month, like every first day of the month. If you choose 31 and February comes around, no task is scheduled for that month because that day of the month that does not exist.

Options

When you click the Options button, the SolidWorks Workgroup PDM Convert Options dialog box appears.

These options are pretty self explanatory. We recommend keeping Latest revision only checked. If it is not checked, all revisions in the selected project or vault are updated.  The other check box, Check if files can be re-opened after update, tells the Task Scheduler to re-open converted files to verify file integrity. If any issues are found, these will be reported, but it does not back out converted files from the vault. Please remember that using this option will obviously increase the conversion time greatly.

Advanced

Click the Advanced button. As you can see, the Advanced Options dialog box for Convert Workgroup PDM Files lets you choose a Task working folder, the Time out (seconds), and Backup task files.

Be sure that the Task working folder that you choose has enough disk space to hold all the files. It is also a good idea to specify a Time out. You can check Run Minimized so that you do not see the SolidWorks window open as it performs the task.

Once you have set all of your options, click Finish.

A dialog box will come up that shows you an estimate of the amount of time required to complete the conversion process. Click Yes to schedule the task. Click No to return to the Convert Workgroup PDM Files dialog box to make changes to the settings or to cancel the task. When you click Yes, the task and its title, scheduled time, scheduled date, and status appear in the Tasks panel. The status of the task is Scheduled. When the task is finished, the status changes to Completed.

Remember that your computer must be on at the scheduled start time. The SolidWorks Task Scheduler window does not have to be open. What if you forget and your computer is off? Well, your computer turns on, then the task will run.

Print Workgroup PDM Files

Do you ever get tired of having to open file, click File-Print, close the file, then open another file, click File-Print, close the file, and so on. Well, if you have a lot of files in the Workgroup PDM vault that you need printed, you don’t have to manually open each one to get them all printed out. All you need to do is to set up an easy batch print task using the SolidWorks Task Scheduler. You can select the complete vault of just one project, filter for file type, and schedule a single job or recurring jobs. The documents are copied to a temporary folder, which you can specify, on your local drive. To get started, in the SolidWorks Task Scheduler dialog box, click Print Workgroup PDM Files.

Log in with your Workgroup PDM user name and password and the name of the computer with the Workgroup PDM vault. You are only prompted for your user name, password, and computer name the first time when you create a Print Workgroup PDM Files task in the current SolidWorks Task Scheduler session. In the Print Workgroup PDM Files dialog box, you can choose from several options. You can select the complete Vault of just one project, filter for file type, and schedule a single job or recurring jobs. The documents are copied to a temporary folder, which you can specify, on your local drive.

First, name your task. The default name is Print Workgroup PDM Files, but you can use any name that you like. Next, click the Add Project button. Only projects to which you have read-write access are displayed. Ask your administrator to enable read-write access to the projects you need to print. Select one of your projects from the list that appears in the Workgroup PDM Projects dialog box. You can include documents in subprojects in the print operation as well. You can add as many Projects as you wish. Every time you use the Add Project button, it adds another project to the list. If you add a wrong project or you change your mind, you can use the Delete button to remove a project from the list. To the right of the Project list is the column File Name or Type. You are given the ability to filter the files in a project based on type: parts (*.prt, *.sldprt), assemblies (*.asm, *.sldasm), drawings (*.drw, *.slddrw), all SolidWorks files (*.sldprt, *.sldasm, *.slddrw), or all files (*.*). You can select a type from the list for each project.

Task Schedule

Whether you need to print your vault files just this one time or on a regular basis, you can schedule this to occur automatically. Task Schedule is a great feature to make your workload easier and to make sure that you do not forget. The Task Scheduler lets you set the schedule. Pick from Once, Daily, Weekly, or Monthly. You can even control the exact start time and date. Keep in mind that SolidWorks Task Scheduler window does not need to be open when the files are scheduled to print, but your computer and printer must be on at the scheduled start time. If your computer is off at the scheduled start time, the task runs when you turn your computer on.

What Printer is Going to be Used?

Most companies these days have more than one printer. So, please make sure that you use the Options button to specify what printer you want to use and any printer other options you need set.

Advanced

The Advanced Options dialog box for Print Workgroup PDM files lets you choose a Task working folder, the Time out (seconds), and Backup task files.

When you are ready to go, click Finish. The task and its title, scheduled time, scheduled date, and status appear in the Tasks panel. The status of the task is Scheduled. When the task is finished, the status changes to Completed.

Export Workgroup PDM Files

In the SolidWorks Task Scheduler dialog box, click Export Workgroup PDM Files.

Log in with your Workgroup PDM user name and password and the name of the computer with the Workgroup PDM vault.

The Export Workgroup PDM file task lets you export files from your vault very easily. First, name your task. The default name is Export Workgroup PDM Files, but you can use any name that you like. Next, pick one of the Export file types. Choose from Dxf (*.dxf), Dwg (*.dwg), IGES (*.igs), Adobe Portable Document Format (*.pdf), STEP AP203 (*.step), STEP AP214 (*.step), and JPEG (*.jpg).

Click the Add Project button.  Select one of your projects from the list that appears in the Workgroup PDM Projects dialog box, and then click OK. You can add as many Projects as you wish. Every time you use the Add Project button, it adds another project to the list. If you add a wrong project or you change your mind, you can use the Delete button to remove a project from the list. To the right of the Project list is the column File Name or Type. You are given the ability to filter the files in a project based on type: parts (*.prt, *.sldprt), assemblies (*.asm, *.sldasm), drawings (*.drw, *.slddrw), all SolidWorks files (*.sldprt, *.sldasm, *.slddrw), or all files (*.*). You can select a type from the list for each project.

Whether you need to export your vault files just this one time or on a regular basis, you can schedule this to occur automatically. Task Schedule is a great feature to make your workload easier and to make sure that you do not forget. The Task Scheduler lets you set the schedule. Pick from Once, Daily, Weekly, or Monthly. You can even control the exact start time and date. So, rather than staying up all night at the office, you can be at home in bed while the Task Scheduler works for you. (Don’t tell your boss! Just let him keep wondering how you get so much work done! If you are the boss, sorry.)

Ever wonder where all these files are going to be stored? Do you have to worry about moving the files around and try to find what went where? Of course not! Just specify a folder where you want the exported files to be saved to. If you have done this before, Task Scheduler remembers the last export location you specified in the current session. You can also copy the files into the Workgroup PDM vault. Since the option is called Copy PDF into vault for View As PDF command, this is obviously only for the Adobe Portable Document Format only. Note that you cannot delete outdated PDFs from the vault, but you can replace them. Using the All drawings, replacing existing PDFs option ensures that PDFs are available and up-to-date for all drawings. The process is very straightforward. So, if you have a bunch of drawings to convert to pdf, you have the option to save the files in a folder of your choice, the Workgroup PDM vault, or both. Speaking of options, click the Options button.

As the Export Options dialog box shows, you can indicate your export options for the export file type you selected back in Export file type. Note: Export options are available for all file types except JPG.  Lastly, there is the Advanced button.

The Advanced Options dialog box for Export Workgroup PDM files lets you choose a Task working folder, the Time out (seconds), and Backup task files.

When you are ready to go, click Finish. The task and its title, scheduled time, scheduled date, and status appear in the Tasks panel. The status of the task is Scheduled. When the task is finished, the status changes to Completed.

We hope this series has given you an insight to how to access the tools in the SolidWorks Task Scheduler. Please check back to the CATI Blog as the Dedicated Support Team will continue posting new series of articles every month that go further into the details of many of the SolidWorks tools. All of these articles will be stored in the category of Daily Dose.....of SolidWorks Support and links to each article with their release date are listed below:

• SolidWorks Task Scheduler - Part1 (Bryan Pawlak 4/2/14)


• SolidWorks Task Scheduler - Part2 (John Van Engen 4/3/14)


• SolidWorks Task Scheduler - Part3 (Blake Cokinis 4/7/14)


• SolidWorks Task Scheduler - Part4 (Neil Bucalo 4/8/14)

Neil Bucalo, CSWP
Certified SolidWorks Support Technician
Computer Aided Technology, Inc.

SolidWorks Task Scheduler – Part 3

SolidWorks Task Scheduler – Part 3

Welcome to part 3 of or blog series covering the SolidWorks task scheduler.

In this section, we will cover the tasks of Convert to High Quality Views, Run Custom Task, Create eDrawings, Update Simulation and the Design Checker.

Convert to High Quality Views:

So why do we want high quality views? Believe it or not, High Quality views make your file sizes much more manageable. Draft Quality views will actually make the file size larger. This is explained in my earlier blog article http://blog.cati.com/2012/10/why-are-some-of-my-drawing-files-so-large.html.

Let's say that you had your SolidWorks setting to create Draft Quality views. All your drawings will be created this way and you may have some very large drawing files. The Task Scheduler is an easy way to convert these all back to High Quality. Converting these is as simple as most of the Task Scheduler tasks. Just select a file or folder and run the task or schedule it for a later time.

Run Custom Task:

You can schedule tasks to run any application, using macros or command-line arguments that you specify.

See SolidWorks API and Add-Ins Help Topics for information about SolidWorks macro files.

Anything that you can run from Windows Start > Run can run as a custom task in SolidWorks Task Scheduler. See the Help files in the application you want to run for information about program command-line arguments and macros in that application.

1. Click Run Custom Task on the sidebar, or click Tasks > Run Custom Task.


2. In the dialog box, type a new title for the task or leave the default in Task title.


3. In Program path, type the path to the program you want to run, or click Browse to locate it.


4. If the program requires any program arguments, type them in Program arguments.

SolidWorks Program argument	Program argument definition	Set by default
/b	Run the SolidWorks software in the background	yes
/m	Run the SolidWorks macro	yes

1. To run a macro or SolidWorks macro template, type the path in Macro file path, or click Browse to locate it. If you specify a SolidWorks macro template, the token names and their types appear in the Parameter Name and Type columns under Task parameters. In each row that shows a Parameter Name and Type, click in the Parameter String column and type the parameter value.


2. If you specify a SolidWorks macro template, create a backup copy of the macro template file before scheduling and running the task, or store the macro template file in a location other than the task working directory. Click View > Options > Task Options to see the task working directory.

Creating a SolidWorks Macro Template

A SolidWorks macro template is a SolidWorks macro that lets you specify parameter values when you schedule it as a custom task in SolidWorks Task Scheduler. A SolidWorks macro template is a text file that typically contains Visual Basic code, SolidWorks API calls, and token names. When you schedule a SolidWorks macro template to run as a custom task in SolidWorks Task Scheduler, you specify the parameter values to substitute for the token names.

Token names can be either text strings or numerics. They are formatted as follows:

Type of Parameter	Format of Token Name
String	$$$<token_name>$$$
Number	###<token_name>###

A SolidWorks macro template must have a .swb filename extension.

To create a macro template:

1. Open a new text file using Windows Notepad, Microsoft WordPad, or other text editor.


2. 
   
   Copy and paste a SolidWorks macro into the text file.
   
   

   See SolidWorks API and Add-Ins Help Topics for information about SolidWorks macro files.

   
   


3. Type token names in place of the parameters whose values you want to specify. For example:

Original code:	swApp.SetCurrentWorkingDirectory "c:\temp"
Modified code:	swApp.SetCurrentWorkingDirectory $$$TASK_WORKING_DIR$$$

1. 
   
   Save the text file with a filename extension .swb.
   
   

   Create a backup copy of the SolidWorks macro template file before scheduling and running it, or store the SolidWorks macro template file in a location other than the task working directory. Click View > Options > Task Options to see the task working directory. When a task using a SolidWorks macro template runs, the system creates a copy of the macro template and replaces the token names with the parameter values you specified when you scheduled the task. The system saves the file in the task working directory under the same filename as the original SolidWorks macro template. If the original SolidWorks macro template is stored in the task working directory, the system overwrites it with the new file.

   
   

See the Task Scheduler help file for a Code example

Create eDrawings

The Task Schedule is a great way to produce eDrawings in quantities.

Simply create an eDrawing task as you would with any other Task Scheduler option.

Once Again, you can select entire folders (with sub directories or individual files)

You Also have the option of what type of files you want to convert (.sldprt, .sldasm,.slddrw)

Update Simulation:

This is one of my favorite tasks. Anyone working with Simulation studies knows that it can take a long time to run some large studies.

Although the Task is described as "Update Simulation", this does not mean that the Simulation Study must have already had been run. You can setup your study and then run the initial run with the task Scheduler.

This is also a great option if you have made a change to a component or any other changed parameters after you have run a study.

Design Checker:

SolidWorks Design Checker verifies design elements such as dimensioning standards, fonts, materials, and sketches to ensure that SolidWorks documents meet pre-defined design criteria. See http://www.solidworks.com/sw/products/3d-cad/cad-standards-checking-and-drawing-comparison.htm for additional information on the Design Checker.

1. Click Design Checker on the sidebar, or click Tasks > Run Design Checker.


2. In the dialog box, type a title for Task title.


3. 
   
   Click Add Standards and select one or more standards files (*.swstd).
   
   

   Drafting standards (ANSI, ISO, DIN, JIS, BSI, GOST and GB) are provided with a set of built-in standard files. The file location of the drafting standards is install_dir\dsgnchk\Data.

   
   


4. Specify files or folders (not both) for Task files or folders.

Option	Description
Include subfolders	Available when you select folders.
Add File	Browse with the Open dialog box for SolidWorks files.
Add Folder	Browse for folders with the Browse for Folder dialog box. Specify part, assembly, drawing, or all types of SolidWorks files for File Name or Type.
Delete	Select an item in the list and click Delete to remove the item.

1. 
   
   Select Auto correct all failures to correct all failed checks for which Design Checker supports autocorrection.
   
   

   

   
   

We hope this series has given you an insight to how to access the tools in the SolidWorks Task Scheduler. Please check back to the CATI Blog as the Dedicated Support Team will continue posting new series of articles every month that go further into the details of many of the SolidWorks tools. All of these articles will be stored in the category of Daily Dose.....of SolidWorks Support and links to each article with their release date are listed below:

• SolidWorks Task Scheduler - Part1 (Bryan Pawlak 4/2/14)


• SolidWorks Task Scheduler - Part2 (John Van Engen 4/3/14)


• SolidWorks Task Scheduler - Part3 (Blake Cokinis 4/7/14)


• SolidWorks Task Scheduler - Part4 (Neil Bucalo 4/8/14)

SolidWorks Task Scheduler - Part 2

Welcome to part 2 of or blog series covering the SolidWorks task scheduler.

In this section, we will cover the tasks of Print Files, Import Files, Export Files, and Update Custom Properties.

Print Files:

Click Print Files on the sidebar, or click Tasks > Print Files.

In the dialog box, type a new title for the task or leave the default in Task title.

Select the files or folders you want to print:

• 
  
  To select files:
  
  
  
  
  • Under Task files or folders, click Add File.
  
  
  • Select the types of files to print in Files of type.
  
  
  • Browse to the file to print, then click Open.
  
  
  • Repeat steps a, b, and c to select additional files.
  
  
  
  


• 
  
  To select folders:
  
  
  
  
  • Under Task files or folders, click Add Folder.
  
  
  • Browse to the folder that contains the files to print, then click OK.
  
  
  • Under File Name or Type, click in the row that contains the folder you just added, then select the types of files to print.
  
  
  • Repeat steps a, b, and c to select additional folders.
  
  
  • If you do not want to include subfolders, clear Include subfolders.
  
  
  
  

To delete a file or folder from the list, click its number in the leftmost column, thenclick Delete.

Under the options button you will find a list of printers and limited page settings.

Import Files:

• Click Import Files on the sidebar, or click Tasks > Import Files.


• In the dialog box, type a new title for the task or leave the default in Task title.


• Select the files or folders you want to import.


• 
  
  Under Task output folder, select one of the following to specify where to store the imported files.
  
  

  **You can schedule tasks to import IGES (*.igs, *.iges) and STEP (*.step, *.stp) files into SolidWorks part (*.sldprt) files.

  
  

  Click the Options button to access Import options similar to SW open menu.

  
  

Export Files:

• Click Export Files on the sidebar, or click Tasks > Export Files.


• In the dialog box, type a new title for the task or leave the default in Task title.


• 
  
  Select the target file type in Export file type.
  
  

  Available selections for target file type:

  
  
  
  
  • Dxf (*.dxf)
  
  
  • Dwg (*.dwg) files
  
  
  • IGES (*.igs)
  
  
  • Adobe Portable Document Format (*.pdf)
  
  
  • STEP AP203 (*.step)
  
  
  • STEP AP214 (*.step)
  
  
  • JPEG (*.jpg)
  
  
  
  


• Select the files or folders you want to export:


• Under Task output folder, select one of the following to specify where to store the exported files:

Update Custom Properties:

• Click Update Custom Properties on the sidebar, or click Tasks > Update Custom Properties.


• In the dialog box, type a new title for the task or leave the default in Task title.


• Select the files or folders for which you want to update custom properties


• When finished selecting files click next.

Add new custom properties or modify existing custom properties in SolidWorks documents.

To specify custom properties to add or modify:

1. Click in the first row in the Name column.


2. 
   
   Select an existing custom property name from the list, or type a new name.
   
   

   Material, Weight, DrawnDate, MakeOrBuy, and CompanyName are a few examples of the many custom property names that are predefined in SolidWorks documents.

   
   

   In a SolidWorks part, assembly, or drawing document, click File > Properties > Custom to see the entire list of existing custom property names for that document. See Summary Info - Custom and Configuration Specific in the SolidWorks Online User's Guide for more information on working with Custom Properties in SolidWorks documents.

   
   


3. Press Tab to move to the Type column, and select a custom property type (Text, Date, Number, Yes or no).


4. Press Tab to move to the Value column, and type a custom property value.

Type	Value
Text	Type any text.
Date	Type a date in mm/dd/yyyy format. For example, enter July 26, 2004 as 07/26/2004.
Number	Type any numerical value.
Yes or no	Type yes or no (not case sensitive).

1. Press Tab to move to the Configuration column. If the custom property that you are adding or modifying affects configurations within the SolidWorks document, type the configuration name. Otherwise, leave blank.


2. Click in the next row in the Name column, and repeat steps 2 through 5 for each custom property that you want to add or modify.


3. Click Finish.

We hope this series has given you an insight to how to access the tools in the SolidWorks Task Scheduler. Please check back to the CATI Blog as the Dedicated Support Team will continue posting new series of articles every month that go further into the details of many of the SolidWorks tools. All of these articles will be stored in the category of Daily Dose.....of SolidWorks Support and links to each article with their release date are listed below:

• SolidWorks Task Scheduler - Part1 (Bryan Pawlak 4/2/14)


• SolidWorks Task Scheduler - Part2 (John Van Engen 4/3/14)


• SolidWorks Task Scheduler - Part3 (Blake Cokinis 4/7/14)


• SolidWorks Task Scheduler - Part4 (Neil Bucalo 4/8/14)