Sunday, 16 September 2018

Solid Edge Video Quick Tip #079

This Solid Edge video tip is about moving or changing balloon position without deleting it.

To reposition balloons on a drawing view along the Alignment Shape, drag the handles. Alternatively, cut-paste balloons and reattach them to the view as shown in this video:

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Solid Edge Video Quick Tip #078

This Solid Edge video tip is about joining two bent flanges together. The Close 2-Bend Corner command can be used to do this and there is NO need to create a tab on the top flange to get that face closer to the left flange.


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Solid Edge Video Quick Tip #077

This Solid Edge video tip is about automatically getting the total length of a copper tube and displaying it in the Bill Of Materials Table.

When creating copper pipes using a 3D sketch, to obtain the total length of the 3D sketch, there is an easy way to get the total length automatically.

You can use the Frame feature in the assembly environment.  You can create the 3D sketch using just lines and no need for drawing arcs. When you create a Parts List for the tube in the Draft sheet, adding the column for Cut Length will give the total length for the tubing as shown in this 1-minute video.



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Solid Edge Video Quick Tip #076

This Solid Edge video tip is about using the Recognize Holes and Recognize Hole Patterns commands in conjunction with the Create 3D, Part Copy, and Scale Body commands.

Unrelated commands like Part Copy and Create 3D have been in existence since the earliest releases of Solid Edge, while ST1 for the first time in the history of any CAD enabled importing dumb geometry and modifying its features like they were created natively. Scale Body, on the other hand, was introduced only recently in ST10. What do these commands have in common?

Well, there is a combo of post-processing commands that render the outcome of these features meaningful. The commands are Recognize Holes introduced in ST5 and Recognize Hole Pattern which was new in ST6. Let's take a closer look at each of these and how the duo recognition commands compliment them.

The following video shows the steps in detail:

[To view the video fullscreen, right click on the video - Copy URL - Paste in a new browser window]


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Solid Edge Video Quick Tip #075

This video tip discusses the following three cases about advanced usage of the Solid Edge Steering Wheel:

1. Moving holes or any feature in a direction set by using existing geometry in the model.
2. Aligning holes in imported geometry which due to the imperfections in its originating program or errors introduced during the import process may not align properly and pose problems during assembling.
3. Moving features, like holes, in this case, to stop short of a certain distance to an existing feature which may not be possible by using traditional methods.

The following video shows the steps in detail:
 Note: This video has a voice-over

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Saturday, 27 January 2018

Solid Edge Video Quick Tip #074

This tip is about temporarily reorienting parts when inserting them into the assembly in Solid Edge.

Parts are often created with an orientation different from their placement in the assembly. After inserting parts in an assembly with the default orientation, it may pose problems with mating them. 

To avoid this, it would be very helpful if parts could be temporarily reoriented, close to the desired position in the assembly. This can be done in the preview area of the Library.

If the preview is not displayed, right click in a blank area between the file names and select Preview...
Check ON the preview and set it to Interactive for both parts and assemblies. Before dropping the bolt into the assembly, rotate it in the preview area.

You can also zoom and pan using the keyboard and mouse button combinations, as shown in the tooltip. 

Now the part is inserted into the assembly, in the same orientation as that in the preview and also mates correctly.

The following video shows the steps in detail:
 Note: This video has a voice-over

[To view the video fullscreen, right click on the video - Copy URL - Paste in a new browser window]



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Wednesday, 24 January 2018

Solid Edge Video Quick Tip #073

This tip is about creating jogs in coordinate dimension overlapping view edges in Solid Edge.

When creating coordinate dimensions, the extension lines often appear very close to part edges. Sometimes, the extension lines may overlap part edges.

To rectify such situations, select the coordinate dimension, Keep the ALT key pressed and click on the extension line. This creates a jog on the extension line.

You can then move the jog, by simple mouse drag.

To create jogs automatically, change the setting in the Dimension style properties.
Open the Styles dialog and select Dimensions from the list.
Select the dimension style and click the Modify button.
Take the lines and coordinate tab.
In the coordinate area, enable automatic jogging.
Start the Automatic coordinate dimension command.

Jogs are now automatically created.
You can further adjust the jog distance and layout, using the handle points.

The following video shows the steps in detail:
 Note: This video has a voice-over

[To view the video fullscreen, right click on the video - Copy URL - Paste in a new browser window]

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Monday, 22 January 2018

Solid Edge Video Quick Tip #072

This video tip is about automatically dimensioning drawing views in Solid Edge.

Solid Edge provides an amazing feature for automatically dimensioning drawing views.

Start the retrieve dimensions command from the ribbon bar and pick the view.

To automatically retrieve dimensions during view creation, change the global setting.

Click the Solid Edge Application button.
Open the Options dialog.
Take the Annotation tab.
Check ON setting for "Retrieve dimensions during view creation".

Now, Dimensions will be created automatically during view creation.

Drag a part from the Library and drop on a drawing sheet.
A single view is created and its model dimensions are retrieved.

You can also create all three views in a single drag and drop operation.

Go back to the options dialog.
From the drawing view wizard tab, check off the option for "Use drawing view wizard, when models are dragged onto the drawing sheet".

Drag a model again from the Library to create all three views in one step.

Models can also be dropped from Windows Explorer, directly on the drawing sheet in Solid Edge. Three fully dimensioned standard views are generated.

The following video shows the steps in detail:
 Note: This video has a voice-over

[To view the video fullscreen, right click on the video - Copy URL - Paste in a new browser window]



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Thursday, 11 January 2018

Solid Edge Video Quick Tip #071

This video tip is about exploding a sub-assembly as a single unit in the E.R.A. environment.

The E.R.A. environment is used for exploding assemblies in Solid Edge. By default you are not allowed to pick a sub-assembly to explode. You must explode one part at a time and this can become time consuming and cumbersome.

To overcome this problem:
  1. Select the sub-assembly in the path finder.
  2. Click Bind in the Modify group on the ribbon bar.
  3. This binds all parts of the sub-assembly together.
  4. Start the explode command and pick any part of the sub-assembly.
  5. The entire sub-assembly can now be picked as a single unit.
  6. Finally, select the sub-assembly again from the path finder and click un-bind from the ribbon.

The following video shows the steps in detail:
 Note: This video has a voice-over

[To view the video fullscreen, right click on the video - Copy URL - Paste in a new browser window]



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Solid Edge Video Quick Tip #070

This tip is about automatically spacing balloons created during Parts List placement in Solid Edge.


When a parts list is created, you can check the option for Auto Balloon on the command bar. This creates balloons for the assembly components, with default properties.

Sometimes balloons can appear overlapping, when they are auto-created.To fix this without having to move each balloon manually, click the alignment shape.

From the command bar, click Properties. Change the minimum spacing to a higher value.

Now all balloons attached to the alignment shape, are spaced properly.

The following video shows the steps in detail:
 Note: This video has a voice-over

[To view the video fullscreen, right click on the video - Copy URL - Paste in a new browser window]


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Solid Edge Video Quick Tip #069

This video tip is about showing/hiding model sketches in drawing views.

When you want to create a data plate for a device, in which the text is cut out, it could run into several problems. When the part is redrawn, it can take a long time to process, due to a huge number of edges, created during the text cutout. 

There are methods for creating texts on a part, which can be shown on draft drawing.

  1. First, make sure you use the Text Profile tool on the Tools tab, to create the text.
  2. Type in your text.
  3. Draw a rectangle around the text.
  4. Exit the sketch.
  5. Create the drawing of the model.
  6. Select the drawing view and click Properties from the Command bar.
  7. From Part List Options, select List Sketches.
  8. Select the sketch and check ON Show.
  9. Update the view.
  10. The text is now visible without creating a cutout feature in the part.
The following video shows the steps in detail:
 Note: This video has a voice-over

[To view the video fullscreen, right click on the video - Copy URL - Paste in a new browser window]





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Wednesday, 10 January 2018

Solid Edge Video Quick Tip #068

This video Tip is about Combining Holes from different hole features.

In synchronous, you can combine identical hole instances from different hole features into the same feature.

The first step is to convert the holes to surfaces or more precisely a face set 
Next run the hole wizard. It will recognizes these 'free' holes and build a new combined hole feature.

This video shows the steps in detail:

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Solid Edge Video Quick Tip #067

This video tip shows how you can automatically dimension sketches as you draw them without having to explicitly use the Smart Dimension command.

When you draw a rectangle or circle, you have to enter dimensions, why go back and add that same dimension? It is possible to dimension the same way you built it.

Just seems a little weird to enter dimensions twice, right...? 
Build a rectangle, put in the dimensions required, and then go back and dimension those same lines.

The Tip: Solid Edge gladly supports this and you need to simply turn on a time-saver option called Auto-Dimension. This command is truly spectacular and here's a quick video.

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Note that you can also set this option in the IntelliSketch dialog on the Sketching tab of the ribbon bar.

 TnT_18_05.png

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Solid Edge Video Quick Tip #066

This video tip shows how to untrim surfaces.

Solid Edge has a Trim command on the Surfacing toolbar but no untrim command to restore a surface back to its original state.

If all the original information is available with the surface, the Copy Surface command can be used to untrim the surface.

This video shows how...

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Solid Edge Video Quick Tip #065

This video tip shows how to hide all centerlines in a drawing view of a assembly containing tubes in one step.

Two methods can be used to accomplish this:
After a view is placed - using a query on the drawing view.
Before a view is placed - changing the global options.

The following video illustrates both techniques:

[Tip: To view the video fullscreen, right-click on the video - Copy URL - Paste in a new browser window]


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