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ST5 introduces Multi-body modeling

Thursday, January 17th, 2013

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.

 

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Integrated Modeling in Solid Edge

Monday, November 19th, 2012
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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.

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Understanding the Steering Wheel

Tuesday, October 16th, 2012news

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.

Accelerate tool design with a few simple surfacing commands

Friday, September 14th, 2012

After completing a 3D model of your design, it may be necessary to design some custom tooling for manufacturing. Solid Edge provides some very simple surfacing commands to aid in the rapid generation of tool design. For example, you may have to design a custom dimple punch or a dimple punch and die set. Let’s assume that you have to design a tool to create the dimple shown here.

For this example, I will just illustrate how you can quickly design the face of the dimple tool. In a new part template, I use the Part-Copy command to insert the sheet metal part containing the dimple.

I will insert this as a construction body.

Notice that I have several other options available to me, if needed, in the Part Copy Parameters dialog.

From the inserted construction body, I can copy the inside faces of the dimple. I select the Copy Faces command from the Surfacing tab > Surfaces group.

I select all the inner faces of the dimple.

I then hide the construction body and I am left with the inside surface.

Next I create a symmetric protrusion which encompasses the surface.

I then select the Boolean command.

With the default subtract option selected; I select the surface as my tool.

I then select the direction that I wish to subtract, or remove the material, from the protrusion.

The protrusion is trimmed from the surface, as shown.

I now have a perfectly matched solid to the inner dimple face. I can now model the rest of the tool.

Using the same procedure I could create a matching die if necessary.

Many users are unaware of the powerful surfacing commands in Solid Edge. As shown above, these simple yet powerful commands can significantly accelerate your design process. If you would like to learn more about surfacing, we offer training in our advanced modeling class (http://www.designfusion.ca//advancedmodelingcourse.php) or you could try the self-paced training course online at http://www.solidedge.com/spt/en/ST5/spse01560/book.html.

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Using Goal Seek to aid in model design

Thursday, July 19th, 2012
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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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Using the mouse to manipulate the model view in Solid Edge

Thursday, June 21st, 2012news

The middle mouse button, or scroll wheel, provides improved model rotation in ST4. You can now select a vertex, edge, or face as the model rotation center. To do this, simply following the steps below:

First you must let the system know that you want to enter the rotation mode. This is achieved by a single click to the middle mouse button (MMB), on an empty space. You will notice the cursor changes appearance. Before you click the MMB your cursor looks like this:

                    

After you click the MMB you cursor will look like this:

  

Notice that the little blue face, indicating selection mode, has disappeared.

You now have three options available to you: 

 

1. Rotate using a position on a face.

  •  - You can now move the cursor over the face shown below. Notice the dark pink dot, indicating that you are in the rotate mode.

 

  • - If you now hold the MMB down, the part will rotate about the dark pink dot. In other words, the dark pink dot becomes your center of rotation.

 

2. Rotate using a position on an edge.

  • - You can move the cursor over any edge. Notice the entire edge highlights.

 

  • - Holding the MMB down allows you to rotate about the edge. In other words, the edge becomes the axis of rotation.

 

3. Rotate using a position on a vertex.

  • - You can move the cursor over any circular edge. Notice the entire edge highlights.

 

  • - Holding the MMB down to rotate allows you to rotate about the vertex of the circular edge. In other words, the vertex of the circular edge becomes the axis of rotation.

 

Note:  Once you have completed the rotation, you are returned to selection mode. You will have to single click to the middle mouse button (MMB), on an empty space, if you wish to perform another controlled rotation.

 

Other handy mouse controls in Solid Edge

 - Pan the view. Press the Shift key while you drag the MMB to pan the view.

 

- Zoom. Scroll the mouse wheel to zoom in and out.

 

Note: The setting for this scroll behavior is found in Solid Edge options_Helpers page. Enable Value Changes Using the Mouse Wheel. If this option is on, the mouse wheel changes the value in a value edit field. Use Ctrl+mouse wheel to zoom in or out.

- Zoom Area. Press the Alt key while you drag the MMB to zoom into an area.

- Double–click the MMB: Fits the view.

 

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