North America's Leading Siemens PLM Partner

Designfusion Blog

Synchronous Assembly Modeling Boolean Commands in ST6

John Pearson - Wednesday, July 03, 2013

The user can now use faces and bodies from other assembly occurrences directly when executing Boolean operations for the “Tool” step such as Union, Subtract, Intersect, and Split.



This enhancement is intended to remove the Inter-Part Copy step during a synchronous in-place activated modeling operation. Not having to create Inter-Part copies accelerates the design process and avoids the necessity of having to save the Inter-Part copies in the PathFinder.

 

Let’s have a look at the following example:



In this example, I have raised the motor up to show that we need to place some cutouts and holes in the underlying plate.



First, I will edit into the Base Plate part from within the assembly. Make sure that the Hide Previous Level command is turned off in the Part environment. 



Next, I select the Boolean Subtract command from the Solids group in the Home tab.


You are prompted to select the target bodies for the Boolean. In this example, I select the base plate part. 



You are then prompted to identify the tool bodies. In this example, I select the motor and the four mounting bolts, and accept the selection. 



If we hide the tool bodies, you can see the result of the Boolean operation.



Remember, this is a synchronous part, so we can easily add a dimension to the inner cutout and increase the size for clearance.


We can also use the Recognize Hole command and easily convert the holes to threaded holes.


This is just one of the many new features in Solid Edge ST6 geared to accelerate your design process, allowing for faster time to market. 


Solid Edge ST6 Offers Multiple Version Installation

John Pearson - Thursday, June 27, 2013

 

Solid Edge ST6 Offers Multiple Version Installation

 

Solid Edge ST6 now provides the user with the ability to run multiple release versions at the same time. This will allow easier testing of new releases prior to putting them into production. The earliest supported version of Solid Edge for multiple install with ST6 is Solid Edge ST4.

 


Solid Edge Multiple Install will not allow certain combinations of the software to be installed together. For example, users will not be able to have multiple versions of MP’s (maintenance packs) installed from the same release version.

 



Users should also not install different 32/64 Bit versions of Solid Edge on the same system.

 

 

 

 

 


Since this new feature is designed for testing purposes, secondary applications are not fully supported with multiple installs. For example, Solid Edge Embedded Client, Standard Parts, Automated Executions, are not supported.

 

In order to successfully install multiple versions of Solid Edge, the user must run a silent install on the latest version. Before running the silent install, a few steps must be followed:

 

1.    When installing multiple versions of Solid Edge, it is recommended that users install the oldest version first, followed by the latest.

2.    Ensure that you install the associated MP for the oldest version prior to installing the second version on your system.

 

3.    Ensure that the user attempting the silent install has administrator privileges.

 

 

Solid Edge Silent Install

 

You can silently install Solid Edge ST6 using the following command. Be sure to enclose path names in quotes if they contain spaces.

 

Note: Do not silently install Solid Edge if you use Standard Parts or Web Parts. These components require the .NET framework, and the .NET framework is installed only when you run setup.exe.

 

C:\>msiexec /i “D:\CM_SETUP\DISK1\Solid Edge ST6.msi”

MYTEMPLATE=2

USERFILESPECXML=”K:\temp\My Docs\Options.xml”

USERFILESPEC=”K:\temp\My Docs\selicense.dat”

INSTALLDIR=”C:\Program Files\Silent Solid Edge\” /qn+

/l*v “K:\temp\mysilentsetup.log”

 

·         The string D:\CM_SETUP\DISK1\Solid Edge ST6.msi represents the fully qualified path to the Solid Edge MSI file. The drive letter D is only an example of the drive letter for the DVD ROM. Your drive letter may be different.

 

·         The MSI property MYTEMPLATE indicates which type template files are to be installed. Ignoring this property defaults the installation to ISO template files.

 

Integer

Value

1

Metric

2

JIS

3

ISO

4

ANSI

5

DIN

6

UNI

7

ESKD

8

GB

 

·         The MSI Property INSTALLDIR is used to specify the installation folder for the application.

 

·         The MSI Property USERFILESPECXML provides the optional installation of a SE Admin file. You should supply a fully qualified path and filename. This file is copied to the Solid Edge Program folder and processed at the end of the setup.

 

·         The MSI Property USERFILESPEC optionally provides a license file that setup copies to the Solid Edge Program folder at the end of the setup.

 

·         The argument "/qn+" instructs the Windows installer to provide NO user interface and alert you at the completion of the setup using a dialog box. Refer to the Windows help system for further information about Windows Installer arguments. Leaving this argument off the command line will display the setup user interface with selections made and fields provided.

 

Note:  If you are using this option, some installations that require user interaction could fail.

 

·         The argument "/l*v" tells the Windows installer to create a log file of important messages, warnings and errors and write it to the location provided, in this example, K:\temp\mysilentsetup.log. Additional information regarding logging options can be found in the Solid Edge readme.txt file.

 

Note:  Solid Edge requires Microsoft SQL Server 2008 Express. Solid Edge setup.exe automatically installs SQL Server 2008 Express, if it does not exist on the machine. The msiexec utility, commonly used for silent install, will not install the SQL Server 2008 Express software. This must be done manually.

 

Note: After you complete the commands on the command prompt and press “Enter” there will be no indication that the install is running. The install will run in the background until complete, in which case it will inform you whether it was successful or not.



Set Active Solid Edge Version

 

When running multiple versions of Solid Edge on a single machine, users will have to decide which version they will want to be active.

 

 

Users will be provided with a SESetActiveVersion.exe tool in order to switch between active versions of Solid Edge.



 

This will be located within the “DVD\Solid Edge\SptTools\SESetActiveVersion” directory on the installation disk. The User Interface provided with the tool will show which major release versions of Solid Edge are present on the system. To activate a different version, select the desired option from the drop down list and click “Activate”.



Uninstalling Multiple Versions

 

Upon completion of your testing of Solid Edge ST6, it is recommended that you uninstall all versions and reinstall the production version from scratch. The possibility of corruption of the remaining versions exists following the uninstalling of only one version of Solid Edge.




Synchronous Hole Recognition

John Pearson - Thursday, June 20, 2013

If you are using the synchronous modeling in Solid Edge ST5 you may have noticed the new Recognize Hole command found under the Hole Command flyout.




This command, specifically designed for imported models with no history, enables cylindrical cutouts to be automatically identified and re-defined as synchronous procedural hole features. It is available in the Part, Sheet Metal and Assembly environment. The user simply has to select the command and select the model. Holes are automatically recognized and displayed in the Hole Recognition dialog.


 




Hole types and sizes are grouped together automatically.


 


A user can choose not to recognize a cylindrical feature as a hole by toggling off the check mark for the feature.



Within the dialog, you can rename the hole features, by double clicking on the default feature name. You can also redefine the hole feature, by applying saved settings or by using the hole options dialog.




Once the user selects OK, to accept the hole options change, a preview of the new hole parameters is shown on the model. The user then selects OK, in the Hole Recognition dialog, to accept the change.



The user can use the Face Selection option to recognize holes only on selected faces.




Pre-selection of a face, or faces, is also supported. You can select a face, or faces, and then run the Recognize Holes command, to perform recognition on only the selected face(s).



The Hole Recognition command allows users to add intelligent synchronous procedural hole features to imported models. Because it’s a hole feature, it also recognizes the user defined pattern created in all hole features, which can be used for rapid placement of bolts or screws in the assembly.


Customizations and Upgrading Solid Edge

Cory Goulden - Tuesday, April 30, 2013
With the ST6 coming one thing is certain…changes are coming.  This next topic will discuss how to transition from ST4 to ST5 (and as well can be used for ST6 upgrades) in relation to the customizations in Solid Edge.
There are certain things that a CAD Administrator can set up for you and share amongst the masses.  If you do not have the luxury of a CAD Administrator, it is very worthwhile to have users share setups.  It would be best if there was only one person setting things up as this keeps everything to a standard.
S
Solid Edge can, quite easily, bring toolbar settings from version to version.  The toolbars can be re-used as it were.  Also to note is the fact that these customized toolbars can be deployed on a user specific basis as well as a base company template type setting.  For instance, a company standard toolbar customization could be deployed and the user would then be allowed to take it from there.  Every company has certain functions that vary from what SE sets up out of the box.  Companies vary as well.  Users vary even further.  It would be worthwhile to invest the time once to set up company templates and environment settings.  If you do it once, there would be years of savings moving forward.
S
The image below illustrates the settings you can set up and take with you from version to version.  Keyboard, Quick access, Ribbon, and Radial Menu options can all be set up.



Screenshot of "Customize" Menu

 

The next sessions we will discuss how to set up everything.  I always like to have the “Previous Window” (in Draft for this example).  These are the steps I would go through.  Open a draft file, although you can do this without opening a file.  Select the down arrow beside the QAT and go to “Customize the Ribbon”.
S


The following dialogue box opens:



Expand the “View” tab on the left and expand the “Home” tab on the right to look like the image below.
S


Have “Previous View” selected on the left and select “Window” from under the home tab on the right and then hit the “Add” button.  It should look like this:
S


Close the dialogue box and you should notice on your Home toolbar that the Previous View icon has been added.  You may be asked if you want to save this if you need to create a new theme or you could save it to an existing customization.

You can also right click and the following menu shows up allowing you to set the options for the new icon:

S

These settings are saved in the following locations in ST5:

Vista/Win 7:

C:\Users\”username”\AppData\Roaming\Unigraphics Solutions\Solid Edge\Version 105\Customization\

XP:

C:\Documents and Settings\”username”\Application Data\UnigraphicsSolutions\Solid Edge\Version 105\Customization\

Windows 7 shown below for reference:



These settings can be shared between different users and computers.  As you can see, each theme is in a different folder and each type of customization (QAT, Radial Menus, Ribbon, ect) is in a separate file.  Because it is external to the install directory of Solid Edge and is not in the registry these customizations traverse updates to the software version.
S
FOR MORE INFORMATION REGARDING TIPS LIKE THESE, PLEASE VISIT US AT THE SOLID EDGE UNIVERSITY.  I WILL BE PRESENTING AS WELL AS JOHN PEARSON AND MANY OTHER KNOWLEDGEABLE SOLID EDGE USERS.

http://www.solidedgeu.com/

Solid Edge Quicksheets

Cory Goulden - Tuesday, November 20, 2012

A “Quicksheet” is a template of drawing views that are not linked to a model. You can then drag a model from the Library tab or from Windows Explorer onto the template, and the views populate with the model.  If you have standard views on a particular size of drawing, for example, you can have the Draft preconfigured to populate itself based on the model you place on the sheet.

You will to need to set up a Draft sheet (but do not use production drawing as the drafting information will be removed upon save) with your views and other items such as Parts Lists.


1. Go to the SE Application button 


2. From the Application menu, choose the “Create Quicksheet Template” command.


3. Save the file to a location and give it a name that easily identifies it.  It is best to place this on a network area other users can get to if it is useful to share the Quicksheet.   It is also best to locate it in a similar area to where the company templates for SE reside.


* Almost all view properties, including general properties, text and color properties, and annotation properties, are maintained. However, some display properties, such as selected parts display, Show Fill Style, and Hidden Edge Style, are not maintained.


Now a Quicksheet template has been created, but how do we use it?


1. Open your Quicksheet template (either through Windows Explorer or if you set up your User Templates and placed the Quicksheets in that location hit New>Quicksheet> and select your Quicksheet).


2. Drag and drop your desired Part or Assy onto the sheet from Windows Explorer or through the Library tab in Solid Edge.


3. Solid Edge will place the geometry and will be ready for the next steps.

Integrated Modeling in Solid Edge

John Pearson - Monday, November 19, 2012

With any new technology, you have your early adopters. This is followed by a general acceptance of the new technology, and of course, you always have your hold outs or late adopters.  Solid Edge ST and ST2 appealed to the earlier adopters for synchronous technology. With ST3, ST4 and now ST5, we are seeing most of our customers starting to use synchronous modeling. This of course has led to many questions. The most asked question is; “Should I use synchronous or ordered modeling?” The answer to this is yes.

One of the unique qualities of Solid Edge is that you are not locked into using synchronous or ordered modeling. Integrated modeling allows you to use both synchronous features and ordered features within the same part or sheet metal model. As a rule of thumb, I encourage users to start with synchronous modeling. If they run into some issues that can’t be addressed with synchronous features, they can switch to the ordered paradigm to complete the model. Let me illustrate this with the following example:

I wish to model the sheet metal cover shown in the following image.

I start in the synchronous paradigm and create a tab, for the top of the cover.

I then add 2 synchronous flanges, in one step, to create the back and left side of the cover.

One of the current limitations, in synchronous sheet metal modeling, is that you cannot drive a flange along a circular edge. Realizing this I will hold off creating the front and right sides until the end, when I will use an ordered feature.

I next use 2 bead synchronous features to create the slots at the top of the part.

I then transition to the ordered paradigm to complete the model.

I use the ordered Contour Flange command to create the front and right face of the cover.

The nice thing about this approach is that it still allows me to modify the model using the synchronous Move/Rotate command.

Live Rules and all the other synchronous editing tools still apply to the model.

As I modify the model, synchronous features update instantly, followed by the re-computing of any ordered features.

For those of you who attended our productivity seminars, you saw this demonstrated live. Other users have learned this process in one of our many synchronous modeling courses, offered over the last year.

This is just one of many examples where Integrated Modeling allows you to benefit from the new synchronous technology, while still utilizing some of the tried and true methods of the ordered technology.  As Solid Edge continues to develop the synchronous features, you may find that you’ll use less integrated modeling. But for now this provides you with a reliable and safe platform to further advance your adoption of this amazing new modeling paradigm we call synchronous technology.

If you’d like to learn more about integrated modeling, you can attend one of our synchronous modeling courses

Editing Part/SM Operations in Assembly

Cory Goulden - Monday, November 05, 2012
In ST5 you can now perform edit operations, from the assembly environment, without first in-place-activating to enter the model directly.  Things you can do:

• Locate, select and edit of ordered features
• Edit synchronous procedural features
• Delete synchronous face-sets and ordered features
• Move face-sets (sync feature) in synchronous parts

Let’s take a look!

Firstly, ordered features are now selectable via the Face Priority select option. (remember hotkey combo is CTL + Spacebar)

Notice in the example below that “Protrusion 1” is available from the Quickpick options in assembly now.


Once selected, “Protrusion 1” has its options displayed for going directly into the features parameters.



Select whatever you would like to edit and SE will take you directly there.  Once complete, just close and return.  This will take you back to where you were in the assembly.

This saves time from previous versions by allowing you to go directly to what you want to modify and brings you back to the assembly reducing the number of mouse clicks.

Editing synchronous procedural features from the assembly level does not in-place-activate the user into the part.  Procedural features are things such as Patterns, Thin wall, Helix, Hem, Dimple, Louver, Drawn cutout, Bead, Gusset, and Etch.  These are editable directly in the assembly.

Using Face Select again, “Louver 1” is selected.
The handle for the procedural features shows up.  If selected we are presented with the following options.

Also, if we were to select the adjacent lover we would be presented with the following options:

Notice that the option to edit the pattern is there.  I know what the usual next question would be “How would I know how to edit the parent of the pattern?”.  Notice the option for “Louver 14”.  If you were to select it, you would be presented with the same options as previously mentioned.



We select “Pattern 1” and now we can modify the parameters that define the pattern.

Once selected, click on the PMI callout “Pattern 2 x 4” and we will get the following options:


Notice we have not left the Assembly environment.
One thing to note about this type of editing: Procedural Feature profile editing requires in-place-activating first.  Also, there is no access to the profile handle from within the assembly.
Happy Edging!

If you would like to learn more about “What’s New in ST5”, stay tuned for our new Update Training course.

Using a Quick Query in Assembly

Cory Goulden - Tuesday, October 16, 2012

Over the years I have noticed some gems in Solid Edge that I would like to share.  Quick Query I feel is a small but powerful little nugget.   I will list the steps below to perform a quick query in assembly and also try to state some benefits to this.  Trust me it takes longer to explain than to do.

Firstly it is important to note that parts and assemblies have properties embedded in them.  These fields should be used for a multitude of reasons from parts lists to searches.  It would be important for all to understand this before moving on.  Obviously these fields must have information in them in order for Solid Edge to report back anything.

Below I have an example part that exists in the example assembly I will use.

To check the properties

We can check what has been entered by going to the part properties.  Select the Solid Edge application button and go to Properties>File Properties.

You can also look at the property manager, which will be discussed at a later date, or perhaps through automation if you have a custom program to assist in entering this data.

 

As you can see below we have an entry of “hardware” in the “Category” field.  This is what we will perform a quick query on later.

We now return to the assembly.

 

Click on the “Select Tools” tab. 

Perform a quick query


RMB in the blank area just below the words in the title bar that say “Select Tools” and the following menu appears.  Note that these options correspond to those fields we had seen in the part properties.  You can set up a search to find these items based on these same categories.


 

You can see the many choices presented to you for searching.  Any one of them can be used.  For this example we will search the “Category” field.

Let’s set up a Quick Query to find and part in the assembly with the word “hardware” in the “Category” field.  We RMB in the blank area, and select “Category”.  This sets the Quick Query option to search the “Category” field in all parts and select and highlight all that contain the word “hardware”.

Once the text has been entered, press the enter key and you should have all the parts highlighted and selected like below:

Note that the highlighted parts are any that contain the word “hardware” in the “Category” field.  This search went into sub assemblies and patterns to select items.  It would also select different items as long as the field had the word hardware in it.   You could do a “Show Only” or other options for the selected set of parts.

There are many applications for this tool (another time we will discuss a full Query).  Quick Query is very useful.  It can select a set of items so you can do things like double check quantities or locations.  Also, because it shows only items matching the query, it can help determine if an item might also be missing properties.  This is good to know especially if those fields are required for a parts list in draft for example.

NX – Create a family of standard parts (Excel)

Charles-Etienne Lavoie - Wednesday, July 04, 2012

                   

                  Design Intent:


                  The most common use of Part Families is to define a standard library part that has many variations.


                  1. Create a hexbolt 

                   


                   

                  2. Rename the expression that you want to keep


                  •   a-Width = the radius of the cap

                    b-Length = length of screw

                  •  

                  3. Define the columns for the Family Table.

                   

                    Choose Tools→Part Families from the main menu bar.

                    Make sure the Importable Part Family Template option is cleared.

                    Click OK on the Warning dialog box.

                    Select the width expression from the top window of the Part Families dialog box.

                    Click the Add Column button.

                   



                    Select the length expression from the top window of the Part Families dialog box.

                    Click the Add Column button.


                  Note:

                  Instead of choosing, Add Column, you could just double-click on the expression name in the Available Columns list, i.e. head_dia.

                   

                    Change the option menu at the top of the dialog box from Expressions to Features.

                    Double-click chamfer from the top list of the Part Families dialog box.


                  Note:

                  The order in which you select the attributes determines the order of columns in the spreadsheet.


                  Tip:

                  In production, you would specify a writable folder for the Family Save Directory, but it is not necessary for this activity since you are not creating Part Family Member files.


                  4.Create the family table.

                   

                  •   Click the Create button from the bottom portion of the Part Families dialog box.

                   


                   

                  •   Type in a few values



                  5.Verify a family member

                   

                    Select a cell in row 3.

                    From the spreadsheet ADD-INS menu bar, choose PartFamily→Verify Part.

                   


                   

                  The NX session becomes active and the family member is displayed in the graphics window.

                    Click Resume in the Part Families dialog box.


                  Warning:

                  The Part Families dialog box may be obscured, if so, click anywhere in the NX window.


                  6.Save the Part Family and the template part.

                    From the spreadsheet menu bar, choose PartFamily→Save Family.


                  Note:

                  The Save Family option internally stores the spreadsheet data within the template part file. It does not save the template part file itself.


                  Note:

                  In order to save the template part containing this newly created Part Family Spreadsheet, you would also choose File→Save.

                   

                  Since we do not use this part anywhere else we are not going to do that.


                  7.Close all parts.

NX – Modeling a tapered thread

Charles-Etienne Lavoie - Friday, May 04, 2012

Currently, the NX Thread command can be used to create a fully modeled straight thread. When
this command is run and the Detailed Thread type is selected a fully modeled thread will be
created. NX provides Modeling tools which allow users to create fully modeled tapered threads.
The Variational Sweep is one of these tools.

 

1. Create a Datum CSYS on the centerline of the thread at the start location of the tapered
thread.

 

2. Create the following expressions in the Expression editor.

 


 

ANGLE will be the included angle of the thread profile. This is typically 60 degrees.
L will be the length of the thread.
P is the thread Pitch which is the distance from thread to thread.
START_DIA is the diameter at the start end of the thread.
TAPER is the taper of the thread.
END_R will be the calculated value L*TAN(TAPER)+STRT_R.
STRT_R will be calculated as START_DIA/2.

 

All expressions should be created as Length type expressions except for the ANGLE
and TAPER variables. These two need to be set to the Angle expression type. If these
variables are not created as Angle type expressions they will not be selectable when
creating the feature.


3. Start the process by creating a Helix curve.

 



The Number of Turns will be calculated by dividing the Length by the Pitch or L/P using
the defined expressions. The Pitch variable will be specified using the expression P.


4. To create the tapered helix the Radius Method Use Law will be used. When selected
the Law Function window will be displayed. At this point select the Linear type.

 



5. Specify the Start and End radius values by supplying these expression variables.

 



Note that the tolerance of the helix can greatly influence the accuracy of the thread.
Initially the helix will be created to the model tolerance in effect when created. This can
be found at Preferences => Modeling => Distance Tolerance.


If the accuracy needs to be improved after the helix is created a higher tolerance can be
specified by editing the helix and changing the tolerance value.


6. After the helix is created select Insert => Sweep => Variational Sweep. Select the helix
curve as the path. For Plane Orientation pick the Through Axis option and select the
centerline of the helix for the vector. For the Sketch Orientation select the same axis.

 



7. When OK is pressed a Sketch will be created. At this point create the profile of the
thread. Constrain all geometry to the point that was created on the helix curve when the
Variational Sweep operation was started. This is an important step.

 



It is significant that the width of the thread be smaller than the Pitch (P-.01). If this width
value is too large then the model will intersect itself as it sweeps along the helix guide
curve. This would cause an invalid solid to be created.


8. When the sweep is complete a hollow thread profile will be created as seen below.

 



9. The thread would be completed by Uniting it to the model of the base of the thread.

 



This same procedure can be used to create a multi-lead thread. When creating the
Variable Sweep Sketch of the thread profile create two threads at half the Pitch in width.
See the sketch below along with the picture of the resultant multi-lead thread. The colors
of the different leads have been altered for emphasis.

 




Using tools provided in NX, users can quickly and easily model complex features.
Randall Waser