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Quicksheets

Tuesday, November 20th, 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.

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Integrated Modeling in Solid Edge

Monday, November 19th, 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. For more information visit our website at http://www.designfusion.ca//synchronous_tech_course.php. New 2013 courses will be added to our schedule soon.

Editing Part/SM Operations in Assembly

Monday, November 5th, 2012handbook
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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