Posts Tagged ‘Synchronous Technology’

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ST5 introduces Multi-body modeling

Thursday, January 17th, 2013api

For long time users of Solid Edge, you already know the advantages of the environmental approach to modeling, instead of the toolbox approach used by other CAD packages. In the environmental approach you create individual parts in separate files and assemble them in a separate assembly file, rather than doing everything in a single file. One of the limits of this approach was that you could only design one body inside of the individual part or sheet metal part file. Yes, you could use the Insert Part Copy command to insert another construction body, but this involved additional steps and forethought in the design process. With ST5 this limitation has been removed.

In Solid Edge ST5 you can now design multiple bodies in a single part or sheet metal file. This eliminates the need to use the Insert Part Copy command, and simplifies certain design processes. In the example below, I’ll show how to use the multi-body modeling to create a simple cavity part.

Assume that I need to create a base for a ball or sphere to sit on. I start by opening up the part with the ball. If the ball doesn’t exist yet I can open a new part and create it.

The next step is to create a base to hold this ball. In ST5 I can use the new Add Body command.

I provide a new name for the new body that I am adding, and click OK.

The initial design body turns inactive (transparent) as I design the new active body.

Notice that once I’ve completed the base feature of the new body, the PathFinder lists both bodies.

The next step is to subtract the ball from the block to create the base holder.

I’ll use the Subtract command and follow the steps.

 

Step 1: Select and accept the target part.

Step 2: Select and accept the tool part.

Design-Body-2 is now a cavity part. I can add features to the part, like a chamfer or round, and paint the part.

I can also publish the parts, using the Multi-body publish command.

I can give the parts unique names and locations and even create an assembly file.

Notice that the newly published parts are linked back to the original part.

Plus an assembly, containing the components, was also created.

This is just one of many examples where the new Multi-body modeling can help you design better. For more information refer to the Solid Edge help documents, or contact us at supp...@designfusion.com.

 

faq

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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Editing Part/SM Operations in Assembly

Monday, November 5th, 2012partner
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

Understanding the Steering Wheel

Tuesday, October 16th, 2012api

Many traditional users have expressed some concern over the use of the steering wheel in synchronous technology. They find it complicated or cumbersome to use. However, once they receive proper training they all agree that it is a powerful and useful tool that is really quite easy to use.

The basics of the steering wheel allow the user to move faces in a linear, rotational or freeform move, similar to the Drag Component command in the assembly environment. The primary and secondary axes allow you to perform linear moves. The torus allows you to perform rotational moves. The tool plane allows you to perform freeform planer moves. With a little knowledge you can quickly and easily move or rotate faces or face sets as required. The notes below are what our trainers hand out, in our courses, and illustrate a few simple ways to control and position the steering wheel.

The steering wheel components

Positioning the steering wheel
When you want to rotate the steering wheel 90° on an axis that is NOT defined by the primary axis of the steering wheel, hold down the Shift key and Click the small blue plane inside of the steering wheel.
  • Shift + Click the Tool Plane will flip the steering wheel 90° about the axis NOT aligned with the primary access.

  • You can also Ctrl + Click the primary bearing knob at the end of the primary axis and key-in an angle.

When you want to rotate the steering wheel 90° on an axis that is defined by the primary axis of the steering wheel, pick the bearing knob on the secondary axis of the steering wheel and drag to rotate.
  • The steering wheel will snap to 90°.

  • You may also Shift + Click the bearing knob at the end of the secondary axis and key-in an angle.

Once you get the steering wheel in the desired orientation, Shift + Click the origin of the steering wheel to relocate it.
  • No need to continue to hold down the Shift key after clicking
  • It will not flip orientation.
  • Secondary axis will not realign to an edge

Changing the Primary Axis Vector

You can change the direction of the primary axis by doing one of the following:

  • Click on any of the 4 positional knobs.

  • Click on the primary bearing, hold the LMB down and align with any keypoint.

For more information on the steering will you can check out the online training section on ‘Moving and rotating faces’ at http://www.solidedge.com/spt/en/ST5/spse01520/book.html or attend one of our synchronous training courses. If you are a regular follower of this blog, you may recall the article on training, where it mentioned that one hour of instructor lead training is equivalent to 16 hours of trying to teach yourself. For more training information please visit our training site at http://www.designfusion.ca//training_schedule.php.
faq

Using Goal Seek to aid in model design

Thursday, July 19th, 2012

The Goal Seek command is one of the calculation tools available for engineering problem solving. It is available in the 3D environments and while drawing 2D geometry in a 2D Model sheet, a drawing sheet, a profile, or a sketch.

The Goal Seek command automates engineering calculations, which can be based on dimensioned geometry, to achieve a specific design goal. Goal seeking finds a specific value for a dependent variable (dependent by formula, for example) by adjusting the value of another variable, until it returns the result you want. Goal seeking shows you the effect on the geometry and it will also update the Variable Table with the new value.

The following is just one example of how to use the Goal Seek command to aid in model creation. This example illustrates how to use the Goal Seek command to help design a sheet metal cover.

Note:  For this example, we have to create a hole pattern, on the top of the cover, to allow for air flow. From previous analysis it’s been determined that we need a minimum open area of 6000 mm². To achieve this we will start by creating a circular cutout and rectangular pattern.

I first create and position a 10 mm radius circle, as shown below, to create our initial cutout.

While still in the sketch environment, I select the Area command, from the Inspect tab > Evaluate group.

I then click in the area of the circle.

I accept the Area by selecting the green checkmark on the command bar.

Next I open the Variable table and locate the Area variable and rename it to Cutout_Area.

 

I also locate the 10 mm variable for the circle radius and rename it to Cutout_Rad.

I then close the Variable table and complete the cutout using the Through All extent option.

Next I create a Rectangular Pattern, as shown below, using the Fit option with the following values:

  • X: = 10
  • Y: = 5
  • Width: = 170 mm
  • Height: = 65 mm

 

The completed pattern should look like the image below.

To prepare to use Goal Seeking I need to create some User Variables. First, I find the X and Y occurrence variables and rename them to X_count and Y_count.

Next I create a Total_Area variable by clicking in an empty row and selecting the area type, from the pull down scroll, as shown below.

I then type in the name Total_Area and tab over to the Formula column. In the Formula column enter the following formula:

                      Cutout_Area*(X_count*Y_count)

 

Note:  I have now created a variable to calculate the total open area created by the pattern. I can now use this variable to help adjust the cutout radius to obtain the desired area of 6000 mm².

To do this I select Goal Seek from the Inspect tab > Evaluate group.

The Goal Seek command bar will appear.

I select the Goal Variable, which is the Total_Area.

I then select the variable that I will allow to change to obtain the Goal variable, which is the Cutout_Rad.

Now I enter in my target value of 6000 mm². (I just have to enter in 6000)

Note:  Goal Seek will now run through a series of iterations, where it will adjust the cutout radius, until it obtains the target value. When it is complete, it will show you the finished model, and post the number of iterations it used and the total elapsed time it took, in the bottom on the Status bar.

If I open the Variable table and view the User Variables, I can see that the radius of the cutout is changed from 10 mm to 12.36 mm, and our total area is now 6000 mm².

Using the Goal Seek command allowed me to determine the optimal radius for my holes without having to do any advanced calculations.

For more practice, try the Solid Edge tutorial on ‘Using Engineering Calculation Tools in Solid Edge.

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Creating insert notches in sheet metal

Thursday, May 17th, 2012partner

Recently I was asked if Solid Edge had a special command for making insert notches in sheet metal. These notches are used to insert tabs or pins in various assemblies. The image below shows a few examples of the type of notches I refer too.

 

To create these notches and others like them, I always use the Bead command in the Solid Edge sheet metal environment. Although designed to create beads, it also creates open ended beads, which are notches. To do this you start with a sketch which represents the length of the bead. For example, I may need a 6.35mm (1/4 “) wide notch, so I create a 6.35mm sketch line.

Using the bead command options, I select the overall shape of the notch. For example, I may need a U-shaped notch 6.35mm high and 10mm wide.

Notice that I set a lanced end condition. I could also use a punched end condition which allows me to extend the cutout portion of the notch.

If this is a feature that I will use often, I can save the settings for easy recall in the future.

Once I say OK to the options dialog, I simply select the direction that I wish to apply the notch.

The resulting bead feature can be edited by adjusting the options or editing the sketch. It can also be added to a feature library.

So my answer to the original question:  “Does Solid Edge have a special command for making notches in sheet metal?” is yes. It’s called the Bead Command.

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