Author Archive

Customizations and Upgrading Solid Edge

Tuesday, April 30th, 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.
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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.
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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”.
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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.
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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:
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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:
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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.
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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/

Quicksheets

Tuesday, November 20th, 2012conditions

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.

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Editing Part/SM Operations in Assembly

Monday, November 5th, 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.  For information related to training from Designfusion follow this link: (http://www.designfusion.com/training_schedule.php) conditions
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Using a Quick Query in Assembly

Tuesday, October 16th, 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.