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Solid Edge University 2014

John Pearson - Monday, April 28, 2014

Join us at Solid Edge University 2014 and Re-imagine What’s Possible

If you haven’t already registered for this annual event, there is still time to join us in Atlanta from May 12-14, 2014. Designfusion will have 5 members of our team present at this year’s event. Three of them will be presenting as guest speakers. This conference continues to grow each year, and this year is no different. This year users can:

    •      - Obtain New Solid Edge Certification
    •      - Learn about the new capabilities of Solid Edge ST7
  •      - Meet the Solid Edge development team
  •      - Network with peers and Designfusion technical experts
  •      - Attend numerous training sessions, and
  •      - Discover a range of complimentary applications from our best-in-breed technology partners.

Attendees will be welcomed at the Westin Peachtree Plaza, in Atlanta, GA, on Monday May 12 with a Welcome Reception from 6 pm to 8 pm. But the real excitement starts on Tuesday May 13, with the launch of ST7. Below are the tentative schedules for Tuesday and Wednesday.

 

 

 

 

You can see that, with this jam packed schedule, the learning potential is huge. This is not a marketing conference but a conference designed to educate users. This is why we call it Solid Edge University. So if you haven’t already registered, there’s still time to do so at http://solidedgeu.com/. We hope to see you there.

An overview of Sensors in Solid Edge

Manny Marquez - Thursday, April 24, 2014

During a benchmark last week I demonstrated sensors. It had been a very long time since I have used that functionality and after seeing the usefulness it could provide for a prospect I decided to write a review for the blog. One such use is when constructing parts and assemblies, you often need to keep track of critical design parameters.


For instance, when designing a shield or shroud that encloses a rotating part, you must maintain enough

clearance for maintenance and operational purposes. You can use sensors to define and keep track

of design parameters for your parts and assemblies.

Types of sensors:

          • • Minimum distance sensors
      • • General variable sensors
      • • Sheet metal sensors
      • • Surface area sensors
      • • Custom sensors
A Sensor Assistant keeps track of sensor alarms that have been triggered by changes
to the model. It quickly accesses the affected sensor definition information so you can
review it and fix the alarm or the model as needed.

You can activate or deactivate the Sensor Assistant and alarm notification
in the graphic window using the Show Sensor Indicator option on the Helpers
tab of the tools options dialog box. This does not affect the operation
of the sensors themselves.

Alarm Types

Displays a bitmap indicating the type of sensor alarm:

  • A sensor violation alarm indicates a design threshold has been exceeded 
  • A sensor warning alarm indicates an element has been deleted:
  • Click the alarm hyperlink to jump to the specific sensor definition information.


We will be using a sample model from the training folder in solid edge.

1. Open the sheet metal assembly located in C:\Program Files\Solid Edge ST6\Training \ (seaabbf.asm) folder.


Minimum distance sensors

Minimum distance sensors are used to track the minimum distance between any two elements.
For example, you can track the minimum distance between two part faces in an assembly.
You define a minimum distance sensor similar to how you measure the minimum distance
between two elements with the Minimum Distance command in the assembly from one part to another.

2. Click on the command, and then select one surface of the chassis part and the other surface from powsup.par part.



3. Enter the name of sensor and values as shown.

4.          

Once done with creating this sensor, we will get back to this sensor on how to trigger the alarm.


Variables Sensors

You can use a general variable sensor to track variables, such as driving and driven dimensions. Let's say that your company only has machines that cuts or bends to a specific size. Ideally you want a safe guard so that you don’t design a part you can’t manufacture or don’t carry stock of that size. In this example we will track the overall height of the part being designed.



5. Edit the Chassis in place.

6. Select the variable sensor. Enter a name for the sensor, then select 552.61 cell. Click on the add variable icon then add values as shown below.

Observe the threshold and sensor range and compare that to the gauge and description. This should give you an idea on how the sensor will alert when it has been triggered.


Sheet Metal Sensor


You can use sheet metal sensors to track design parameters, such as the minimum distance between particular types of sheet metal features and part edges. You can create your own sheet metal sensors from scratch, or you can select from a list of predefined examples. Let’s say that we need to make sure a cutout does not get to close the outside edge, for reason that the heat sink will get hot and damage the component. Sheet metal sensors are available only in sheet metal documents.

7. Click on the sheet metal sensor; make sure to select the Face on the options on ribbon bar. Select surface on part as shown.


8. Select cutouts on (edge set 1) and exterior edges from (edge set 2). Set threshold at 20, therefore if a hole gets 20mm of an edge, a sensor will be triggered.

9.  

Notice the two sensors now; we are done creating this sensor, we will get back to this sensor on how to trigger the alarm.

Surface Area Sensor

You can use a surface area sensor to monitor a surface or a set of surfaces. Also you can monitor both the positive and negative surface area. A negative surface area sensor monitors the "holes" or internal boundaries in a surface.For instance, you may need to track the total area for a series of ventilation holes and cutouts in a surface.

10. Click on surface area sensor icon; select the negative area with face option then click on surface of part as shown.

11. Enter sensor name, with indicated values, again study the current value to the threshold and sensor range. Notice on the airflow gage how much it’s left to trigger the alarm.


Done with creating this sensor, we will get back to this sensor on how to trigger the alarm.

Custom Sensor

You can use a custom sensor to monitor any numeric result that is calculated from a custom program. For example, you could create a custom program that assigns a manufacturing cost to each feature type used for creating sheet metal parts. The program would then monitor the part features and give you the part cost of the completed model.

Note: you need to run the CustomSensorRegistration.exe from the custom sensor folder.

12. Select custom sensor then click on GetMass.



13. Note: If you did not add a material type, you will get this message. Simply go to the material table and add a material. See below.



14. Enter the sensors name and fill in the indicated values as shown below. The current value is 8.18 lbs, we set a threshold of 10 lbs and range between 5 lbs to 15 lbs. If the part goes over 11 lbs the sensor will set a warning alarm.

15.



Let's put all sensors to the test, starting with the clearance sensor, this will allow us to have a minimum distance from other parts on the assembly For example, if you don’t want the heat sink to get any closer to the side wall for it want allow proper flow.


16. Edit in place chassis.psm part. Select Hole 5, then click on dynamic edit, select dimension 62.50 and enter new value of 80. Since the sensor is a Assembly part, you need to (close and re-run) notice the sensor violation alarm indicates a threshold has been exceeded. (If don’t see indication, select on the tools tab click update all links)



17. Click on sensor violation alarm, for sensor details.


In real scenarios you will determine what actionsare needed to resolve the violation by making changes to the model.

In the following scenario we will only be triggering off the sensors to show sensor violations.


18. The following sensors will take place on the part environment (chassis.psm); we will trigger the Height sensor this time. Select the (contour flange 1) then click on dynamic edit. Enter 200mm value to see violation. Click on update all links.



19. We will trigger the holes to edge sensor now, select on the (Cutout 1) click on dynamic edit. Select dimension 30 enter new 15 value then enter.



20. Next will be the Airflow sensor, select on the (Cutout 1) click on dynamic edit. Click on the 94 dimension, enter 90.




21. The final sensor to trigger is weight, Select the (contour flange 1), then click on dynamic edit. Select value 250, and then enter 400.

22.


I hope this simple example on sensors gave you an insight on the usefulness of sensors during design.

Until next time!

Regarding Keyshot?…All I can Say is WOW!

Cory Goulden - Wednesday, April 09, 2014
I have taken the time to learn the rendering portion of Solid Edge. Although it does a good job I found myself learning a lot of new phrases and terminologies that to me, at least, were very specific to the job of someone who may be rendering as a profession.

I admit I have never really paid much attention to rendering as a mouse jockey in the Cad field. I thought though that we have an opportunity to use the 3D model for yet another purpose and so, as SE as my tool, I trudged forward. I was able to accomplish making renderings for presentations, animations for demos to potential customers and a few other things but it seemed to be a little cumbersome and the learning curve was a bit long. This was good. Not great but good.

 

 


Enter a product called Keyshot. Now I am going to do my best to not make this sound like a sales pitch. This product is great, reasonably priced, and learning it is easy enough even I could do it!

A few key points to Keyshot;

The rendering is CPU based. This means a computer that has many cores benefits and does not require much more than that for hardware. It also pauses, renderers in real time, and instantly stops if the CPU/resources are required elsewhere. Start it, go about your business, or go for lunch…whatever. It does a fantastic job at taking care of itself with no interruption to the user.

 

 


To apply material to a model you only need to pick the material and drag and drop it onto the part (as illustrated in the picture above. It will also save this setup information and combining this with “Live Linking” Solid Edge models can be changed and the render settings are maintained. As for modifying the model, you can easily move between Solid Edge and Keyshot with the press of a button and all previously setup information will still be there. How great is that?

The ease of use for creating animations is great too. If you just want to tumble a model, explode and rotate, or whatever your needs may be there is a wizard to walk you through the setups. If you want to off that trail you are free to set up anything you want. Keyshot and the 3D models from Solid Edge can provide a symbiotic relationship that will provide great results without changing anything you already have. You can even embed them as HTML in webpages. You can even create iBook widgets!

 

 


You want a way to be more productive and have a way to better display why your product is the best choice? There are so many ways people are communicating that we all have to try to present the information in as clean and as effective as possible. Combining Keyshot with Solid Edge will do that for you.

www.designfusion.com/keyshot.html

Feel free to contact us regarding any additional questions you may have. We are always here to help.

And, as always, happy Edging!

Constraints and how they work in ordered and synchronous modelling

John Pearson - Thursday, April 03, 2014
There seems to be some confusion amongst some users regarding the ability to constrain synchronous parts. The confusion has even lead to inaccurate information being perpetrated as truths, by some competitive product’s resellers. So I’d like to set the record straight and clear up several misconceptions. First and foremost, you can constrain synchronous models. Secondly you can use the variable table to drive synchronous models. And last, but not least, you can automate synchronous models through custom programming or a configurator.

Ordered constraints


To understand how this works, let’s fist look at an ordered part. Below is a sketch for a part that I wish to model. Notice that I have fully constrained the sketch.

 

 


The sketch has zero degrees of freedom, so I can predict what will happen when I make a dimensional change to any of the 3 values. I control part of the sketch with geometric constraints, which include the following 2D relationships:

 

 


When I use the sketch to create a model, the sketch becomes the parent of the solid model, as shown below:

 


This model is considered constrained because it is controlled by the fully constrained sketch and the depth dimension, added during the extrusion command. Notice that we can go into the variable table and apply specific names to each dimensional variable.

 

 

 

I can now drive predictable model changes using the variable table. Furthermore I can link the variable table to an Excel spread sheet, a custom program, or a configurator to drive model changes.

When a variable is changed, the system first re-calculates the sketch and ensures that the sketch is still a valid profile. It then moves on to the child of the sketch, in this case the model, and re-computes the model to ensure that we still have a valid model. If additional features were added to the model (like a round or chamfer) it would continue to re-compute the next feature(s) until it has completed the feature tree list. For small models with few features, this is a rapid process. However, the more features an ordered model has in it, the longer the re-compute time will take.

Synchronous constraints

Now let’s make the same part in the synchronous mode. We start by making a sketch, as shown below:

  


Notice that I can fully constrain the sketch in synchronous mode. The difference here is that when I create the solid, only the dimensions are migrated to the 3D model. The 2D geometry and 2D geometric constraints are left in the Used Sketch header on the PathFinder. In other words, no parent child relationship is created between the sketch and solid, and the 2D dimensions are converted to 3D driving dimensions on the model, shown below:

 

 


Notice that 3 of the 4 dimensions are red in colour, while the depth dimension is blue. A red colour means that the dimension is locked and can only be modified by a direct edit of that dimension. Let’s make the fourth dimension locked as well.

 

 


So now we have the dimensions fully constrained or locked. What about the geometric constraints? Since the 2D geometric relationships have not been transferred to the model, a lot of users become concerned that the model is no longer fully constrained. They are partially correct. Let’s take a closer look at the model.

By the nature of the solid, we can make a few assumptions.

1. The connect relationships will be maintained at the model level. Why? Because if they are not we no longer have a solid.

2. Synchronous edits use Live Rules, and Live Rules will maintain most of the pre-existing geometric situations. For example, if you attempt to change the values in the part, default Live Rules will keep the walls in their current horizontal/vertical position.

3. Synchronous will only analyze the effected faces in any move. Therefore it only has to re-compute faces affected by an edit.

Even with these assumptions, there admittedly could be some un-expected results if you are using this model in a custom program or configurator. So how do we eliminate potential un-expected results? We use 3D geometric relationships.

Persistent (3D) relationships

 

Looking at the original sketch of our model, you’ll notice that the sketch was centered on the base coordinate system. I can do the same with the model by using the horizontal/vertical persistent relationship command. I’ve placed these relationships in the model, shown below. Notice that they also are listed under a Relationship header in the PathFinder.

 

 


Simply by placing these two relationships, I now have predictability in any dimensional edit. I can now set this synchronous model up in the Variable Table.

 

 

 

I can now drive predictable model changes using the variable table. Furthermore I can link the variable table to an Excel spread sheet, a custom program, or a configurator to drive model changes.

For more complex models, synchronous offers even more 3D geometric relationships.

 

 


Notice the striking similarity between our 3D geometric relationships and our 2D geometric relationships. There is however one big difference. I only have to use the relationships that I need to control my model. Because synchronous technology only re-computes faces that are affected by an edit, I may not have to fully constrain a model.

Some will argue the fact, but the truth is the majority of ordered models that I see from customers are under-constrained. Because of the parent child nature of ordered modelling, this could be, and often is a problem when editing ordered part models. If you doubt this statement, go back to your database and open some of your existing models. Under the Solid Edge options > General tab, turn on the ‘Indicate under-constrained profiles in PathFinder.

 

 

 

If a red pencil icon appears anywhere in the PathFinder, you have under-constrained features.

 

 


This is a real concern in ordered modelling, but not in synchronous modelling. As you’ve seen, the nature of synchronous modelling puts the focus on only what’s being edited. As you have also seen, a synchronous model can be fully constrained if necessary. Either way you can have complete predictability of the model and use it in configurators or custom programs.

So, as I stated at the start of the blog article, you can constrain synchronous models. You can use the variable table to drive synchronous models. And you can automate synchronous models through custom programming or a configurator. Anyone who tells you different has not been properly trained in synchronous modelling or works for a competitive software package.

If you would like more information on synchronous technology or would like to attend one of our synchronous training sessions, please contact us at sales@designfusion.com or visit our training web page at http://www.designfusion.ca//technical-training.html.

How to Create a Rod That Has Bends in Two Directions

Cory Goulden - Monday, March 31, 2014

I have received a few calls lately regarding this subject so I thought I would provide a walk-through on how to make something like the drawing below. This will be one of the rare times I prefer to model in Ordered.




The first step is to understand that we will have to let the 3D system do most of the work for us. We will, like all good trouble-shooters, work out what we know. On one plane create a sketch of the top profile. Then on the corresponding plane create a sketch of the side profile.

Once this is complete we will use some surfacing tools for the second step. Go to the “Surfacing” tab and select the “Extruded” command in the “Surfaces” group.

Once the command is selected ensure the option to “Select from sketch” is selected. We then will need to select one of the earlier selected sketches. Once selected we will ten need to extrude the surface. The extend distance need to be further than the entire profile for the other sketch.


Do the same procedure for an extruded surface from the second sketch. Be sure both surfaces overlap each other after they are completed. You can always go back and adjust any extents after.
Once complete you should have the result similar to what is illustrated below. (I have hidden the sketches for clarity)



From here we will go back to the Surfacing tab and use the “Intersection” command under the “Curves” group.



This command asks us to select the 2 elements. Firstly select one of the surfaces and accept. Next step is to select the second surface and accept.



You will now have a 3D path that you can use for a lofted protrusion.

You can use another command called “Cross Curve” to accomplish the same thing but to understand the concept and break it down a bit I chose to illustrate this methodology. Feel free to use the Command finder for further information.

Once you have created a Lofted Protrusion using this curve as a path you will end up with this;



We have created 2 extruded surfaces, used Solid Edge to create an intersection curve, and then used that curve for a lofted protrusion.

 

I hope this has been useful and Happy Edging!

There’s a CAMWorks for Solid Edge?

John Pearson - Tuesday, March 25, 2014

Last year at Solid Edge University (SEU2013) I was introduced to CAMWorks from Geometric. What I had always considered a competitive product was now being offered as an add-on to Solid Edge. Being a long time NX CAM user, I was a little surprised that Solid Edge would partner with another CAM package, especially one so closely linked to another CAD package. At my company’s request, I put aside my skepticism and started to find out what I could about this new offering.

The first release of CAMWorks for Solid Edge was limited to 2.5 and 3 Axis Milling and Turning. Since most CAM packages can easily handle this type of manufacturing, I focused on what made CAMWorks unique, and how it worked with Solid Edge. Three distinct factors stood out for me during my initial analysis of the product:

    1. CAMWorks for Solid Edge is embedded and fully integrated into Solid Edge.

 

When you install CAMWorks for Solid Edge, it becomes part of Solid Edge. A CAMWorks ribbon is created, and a CAMWorks edge bar is added to the PathFinder.

 

 

This eliminates wasted time and potential errors in loading your Solid Edge model into external CAM packages. Plus you can easily switch back and forth between the CAD and CAM ribbons, to make associative edits or revisions.

     2. CAMWorks for Solid Edge utilizes feature-based machining to allow for rapid tool path generation.

CAMWorks for Solid edge utilizes automatic feature recognition and an advanced database to create some truly impressive knowledge based machining. Once setup the basic workflow is as follows:

 

    - Identify the parts for machining

 

     

     

 

    - Extract features to be machined

 

 

 

    - Generate the Operation Plan (utilize the database to determine how the features are to be machined)

    - Generate the toolpath

 

  

 

 

 

    - Simulate/Verify the toolpath

 

 

 

 

 

    - Post process to create the G-code

 

 

 

If the database is setup correctly, each process is automatic. I’ve seen situations where you can go from CAD model to G-code in 5 button clicks, if you skip the simulation step.

 

    1.      3. CAMWorks for Solid Edge can be customized to meet the individual needs of each company.  

 

The database (TechDB) used in CAMWorks for Solid Edge, can be set up differently for each company and even each user. This allows companies to capture and reuse their best machining practices, saving time and eliminating repetition. It should be noted that you can create operations on the fly and save them to the database, allowing you to continually expand and improve your knowledge base for future machining.  The potential exists to reduce programming time from hours to minutes, but it does require some up front effort to realize this kind of result.

Despite these impressive points, I wanted to learn more about future plans for the product. Two weeks ago, I was invited, by Geometric, to attend a training session for VAR’s in Scottsdale, Arizona. I eagerly accepted the invitation, mainly to escape the brutal winter we’ve been having, but it also gave me an opportunity to get answers right from the source.

I was not disappointed; the temperature ranged between a balmy 25-28 degrees Celsius, and the capabilities of CAMWorks exceeded my initial expectations. They have recently added Multi-Axis milling, Mill-Turn, and Wire EDM capabilities and continue to work with Solid Edge to improve the product.

As a combined result of my investigation, and the work of our management team, we will be adding CAMWorks for Solid Edge to our product line. We believe this will complement our existing products, and provide more choice to our customers. We will be adding more information to our website, as it becomes available, and have plans to offer training in the future. In the meantime, if you’d like to learn more about CAMWorks for Solid Edge, please contact your account manager or contact us directly at sales@designfusion.com.     

        

How to Model an Airfoil

Manny Marquez - Wednesday, March 12, 2014
Last week, on my flight back to Chicago, I always find it more enjoyable for long flights especially to have the window seat for a few reasons. Of the few things that I enjoy, one is watching how thrust is pushed in between the turbine blades of the engines and how the wing flaps pivot when used for breaking as the plane lands.

When I had landed, a thought came to me; and that was that I have never seen a turbine engine airfoil blade or wing model in Solid Edge. So I took it upon myself to do some research on how I would model airfoils. I came across some interesting web sites that explain the whole explicit mathematical functions used for 2D curve definition for airfoil design; very fascinating however, I just wanted the basics.

 

 

 

Here is the basic anatomy of a blade; you have root type, root width, root height, and airfoil height.


For many years, research and studies have been conducted on airfoil blades and also on the performance of wing design aerodynamics. Shown below is an airfoil generator for blades that I found online.

As you can see by entering the appropriate values you should be able to generate an airfoil based on you requirements.

Geometry Airfoil Generator Example: 

 

 

After generating the foil you have two options, either to create a DAT file or simply copy and paste the X,Y,Z coordinates to your excel.

I chose to just simply copy and paste directly to Excel. Notice A=X B=Y C=Z, in some cases if you are creating a simple airfoil you may only get XZ coordinate values. If that is the case you need to insert a cell and enter zero for Y as shown in this case.

 


 

 1. Before you start anything you will need to model up the root type, make this part in ordered. Surface modeling works best on the ordered mode. I downloaded a CAD model from GrabCAD website. If you have the time to model, a basic shape like shown below, make sure the XYZ origin is setup correctly. Therefore, when creating the airfoil via the Solid Edge curve by table option, it is placed correctly on the root top surface.

 

 

2. Next click on the curve by table option. It is located in the surfacing tab on the curves group.

 

 

3. Click on browse, then find the excel files.

 



4. Select finish. Notice the 2D airfoil automatically sets on the origin.

 

 

5. By clicking on the edit points data step, the Excel sheet will open. If there should be a need to modify the XYZ points manually you will be able to do so at this step. Click finish when you are satisfied.

 

 

6. Another option is to set the curve fit and curve end conditions.

 



7. On the next step, we are going to create two User coordinates systems.
Under the surface tab, find coordinates system on the planes group. This will allow us to place new airfoils at any point in space.

Select (key-in (relative to another Coordinates system)

 



8. Enter 3 on the (Y), next then preview and then finish. Repeat the same step for the second UCS, except enter 6 for (Y).

 

You model should look like this.

 

 

Now, we can continue since we have created the UCS to place the airfoils.

9. Repeat the same steps for the second airfoil. You may have as many airfoils as you wish- usually that varies on how
complex your blade may be. For this example, I will only be using three airfoils.

 

10. This time before clicking on finish, select the second coordinate system (the names may vary).

 

 

Repeat for last Airfoil.

 

 

Your model should look like this: Root with all three USC in place.

11. We are now going to create a BueSurf. This will create the outer shell for each airfoil, thus creating the turbine blade.

12. Click on the BlueSurf command, located on the surfaces group.

13. Select the first airfoil sketch.

 

 

 

Make sure the cross section vectors are consistent with the other geometery.

14. Select on the second airfoil sketch, notice again the vectors are consistent with the first selection.

 

 

15. You model should look like this.

 

 

16. Continue on with the selection

 

 

The overall blade has been constructed, we will now add rotation to the blade. Some blades have more complex geometry, I’m only using three airfoils to crreate a simple blade

17. Select the origin, and then click on edit definition.

 


 

 

18. Click on the orientation step.

 

 

19. Enter 25˚ for the Y direction.

 

 

Notice the foil is now 25˚ about the Y

20. Repeat the same step for the last coordinate system. Enter 30˚

 

 

21. You have completed this turbine blade using a geometry generator with BlueSurf. I hope you enjoyed it.

Did you know that you can do this in Solid Edge . . .

John Pearson - Tuesday, February 11, 2014

Did you know that you can do this in Solid Edge . . .

As a support team member, and technical trainer, part of my job is to learn the technology inside Solid Edge. Therefore, I’m allotted time to learn, test and research the latest technology. But as I’m sure many of you will agree, this is a privilege most users don’t have. Users are under the gun to meet deadlines and therefore often stick to what they know, even if it’s not the most efficient approach.  As a result many users are unaware of the full potential of Solid Edge. 

On more than one occasion I have received requests for custom programming for capabilities that already exist in Solid Edge. I often find myself saying “Did you know that you can do this in Solid Edge already”. With this in mind I thought it might be a good idea to start recording some of these moments and share them in our blog. So below are some of the questions I get from our customers along with how to do it in Solid Edge.

I have to delete a part list from my draft file, is there a quick way to delete all my balloons, or do I have to pick them individually?

Did you know that you can do this in Solid Edge using the SmartSelect command? To select all the balloons at once do the following steps.

- Pick the Select tool to launch the Select tool command bar.

 

   

            

  • - Select the SmartSelect icon from the Select tool command bar.

 

 

  • - Select one of the balloons from your view.

  • - The SmartSelect Options dialog box appears.  Check Element type and click OK.

 

 

 

 

 

  1. - Notice that all the balloons highlight.
  2. - Hit the Delete key and they are all deleted.
  3. The SmartSelect command searches the active sheet for other elements with similar attributes, such as element type, color or line width. All matching elements are automatically added to the selection set. Now you can make changes to the selected elements all at once. This is ideal to make changes or delete dimensions, lines, callouts, etc. in the Draft environment.
  4. I have a large assembly and when I’m zoomed in and try to rotate the part, it flies off the screen. Is there a better way to control the rotation? 
  5. Did you know that you can do this in Solid Edge using the middle mouse button? The problem here is that the default center of rotation is (0,0,0). So if you are zoomed in, away from the origin, any rotation appears to rotate out of view. What you need to do is change the center of rotation by following these steps:
  6. - Zoom into the area you want to view.
  7.  
  8.  

     

  9. - Click your Select tool. Notice that the cursor has a small gold box beside it.
  10. - Click the middle mouse button, in an empty space, and the gold box will disappear.
  11. - When the gold box disappears, move the cursor over the model. Notice the bright pink dot attached to the cursor.
  12. - This bright pink dot represents the center of your next rotation. Move it to where you want the center of rotation to be, and then hold down your middle mouse button to rotate.

 

 

  1.  
  2. - Notice the rotation symbol on the cursor, and that you are rotating around the pink dot.

 

  1. When you release the middle mouse button you are placed back into selection mode. You can also use this in the part or sheet metal environments. For more information, and additional mouse tips, read the Solid Edge Help docs under the “Using the mouse” heading.
  2.  
  3. I want to place a dimension between two points that are not horizontally or vertically aligned.
  4. Did you know that you can do this in Solid Edge using the Distance Between command? All you have to do is follow these few steps:
  5. - Select the Distance Between command.
  6.  
  7. - On the command bar, change the Horizontal/Vertical option to By 2 Points
  8.  
  9. - Select the 2 keypoints and place the dimension.
  10. For more information, and additional options, read the Solid Edge Help docs under the “Dimensioning overview” heading.

 

These are actual questions that I have received many times from our user base. It just goes to illustrate that Solid Edge is not always being used to its full potential and that there is always room for improvement. The more you understand about the software the more efficient you will become. I plan to continue sharing the more popular questions, from our tech line, in future blogs. If you are a customer of Designfusion’s, and have a question, please don’t hesitate to call our tech line at 1-877-215-1883 or email us at support@designfusion.com.

  • Join us at Solid Edge University 2014

    John Pearson - Friday, January 31, 2014

     

    Siemens PLM Software has announced that this year’s Solid Edge University will be held in Atlanta, Georgia on May 12-14, 2014.  For those of you who have not attended this conference, you are truly missing a great opportunity. Not only do you get a preview of the next release of Solid Edge, but you get to connect with the Solid Edge developers and provide input to the direction of future development. You can also participate in hands-on learning, attend presentations given by CAD users and meet with experts from all aspects of the design continuum. Focus areas will include CAD, design data management, simulation, manufacturing and a host of complementary applications to help you design better. Some of us at Designfusion will be presenting again at this year’s conference.

     

     

    This is also a great opportunity to visit with our sponsors and technology partners and learn new ways to enhance the power of Solid Edge. Many partners are set up at the conference, ready to answer any questions you may have. Plus there is no better place to network with other Solid Edge users who make up this vibrant user community.  I personally spoke with the Designfusion customers who attended last year event and everyone said that the learning experience was well worth the cost of the conference.

     

    I hope you can join me and my colleagues at the Solid Edge University 2014. For more information, and to take advantage of the early bird registration, go to the Solid Edge University website at http://www.solidedgeu.com/.

    Using the Improved Drawing View Wizard in ST6

    John Pearson - Thursday, December 26, 2013
    As more and more users migrate to Solid Edge ST6, I am receiving more calls asking about the Drawing View Wizard. There was a major overhaul in ST6, but do not panic, for you can reset it to behave as it did in previous versions. The new method utilizes the toolbar approach which is found in most Solid Edge commands, where the old way uses the wizard approach.

    How to set the drawing view command to the wizard method

    A new tab has been added to the Solid Edge options in the Draft environment. The tab is entitled Drawing View Wizard, and allows you to define some default settings.

     


     

    To learn about the other settings, click on the Help button. The help documents have a complete breakdown of all the other settings.

    Using the new Drawing View Wizard method

    If you leave the previously mentioned option checked, you will use the new simplified workflow for placing a drawing view. The simplified mode reduces the number of steps required to generate drawing views. It omits the wizard dialog boxes and instead displays the View Wizard command bar at the drawing view placement step. This is the default mode for the View Wizard command.


     

    In the image above you can see that after I selected the part file and I am given a Front view of the part, attached to my cursor, along with a command bar. In this example I am using the horizontal command bar. I could also use the vertical command bar as shown in the following image.

    Note: You can choose whether you want to use vertical or horizontal command bars in the Solid Edge options, under the Helpers tab.

     


     

    I can place this view on my draft sheet and I am immediately put into the principal view command. This allows me to place alternate companion views based on the position of my cursor. For example, if I want a Top and Right view, along with the Front view, I simply move my cursor up and click for the Top view.

     

     

     

    I can then move my cursor to the right and click for the Right view.

     

     

     

     

    To exit the command I hit the Esc key, on the keyboard.

    Preselecting layouts and presetting options

    Before I place any views I can preselect layouts or preset some options. All these options are on the command bar. The image below is that of the vertical command bar. I use this for training because it shows the option names.


     

    As you can see there are over a dozen options here. I will focus on the 6 most common, but a description of all the options can be found in the Solid Edge Help section.



    Drawing View Wizard Options   

    This option allows you to specify content and display options based on whether the drawing view is an assembly, part, or a sheet metal model. When you select it the following dialog appears:


    •    For Part or Sheet metal files.

     

     


    •    For an Assembly file.

     

     


    For those of you familiar with the old Drawing View Wizard, you will recognize these dialogs as the first dialogs that appear. All the options that you are used to are still here.

    Drawing View Layout  

    This option allows you to select additional views to place along with the primary view. You also can change the orientation of the primary view. When you select it the following dialog appears:

     

     


    Once again this dialog should be familiar to existing Solid Edge users. It is a combination of the 2nd and 3rd dialogs of the old Drawing View Wizard. Here you pick your primary view and the companion views. Note that the primary view can be a preset view or a custom view.

    View Orientation

    This option allows you to change the view orientation before you place it. For example, if you just wish to place a single view, you can control the orientation by selecting this option and choosing from the following drop down list:

     

     


    You can use this option if you don’t plan to add companion views.

    Best Fit, Set View Scale, Scale List and Scale value

     

     


    These options allow you to control the size of the view that you are placing. They are identcal options that you would find in the previous Drawing View Wizard command, and are used the same way.

    Saved Settings

    This is a new and very useful option to ST6. It allows you to save your layouts for reuse in other draft files. For example, if I always place a flat pattern of my sheet metal parts, I can place my first layout and save it. To do this I do the following steps:

    1.    Start the Drawing View Wizard command and select the file that I want to place onto the draft sheet

     

     

     

    2.    Set the Flat pattern option.

     

     

     

    3.    Select the scale that I want to use. But do not click to place the view yet.

     

     


    4.    In the Saved Settings dialog I name this layout as Flat and hit the save icon.

     

     

     

    5.    Place your view.

     

     


    The next time I run the Drawing View Wizard, with a Sheet Metal part that contains a flat pattern, I just have to select “Flat” from my saved settings.

     

     

     

    Following the same steps I could save another layout showing the Front, Top, and Right view for the same model, and save it as “FTR_view”. The next time I run the Drawing View Wizard on a Sheet Metal part, I could select from either layout.

     

     

     

    Note: I find saving layouts easier if you always start with a new draft file, per layout.
    There are a couple of things to note here.
    •    To use a saved setting, that setting has to be selected before the drawing view is placed on the drawing sheet.

    •    Your saved settings are based on model type and model size. For example if I place a part file, I will not see the Flat or FTR_view saved setting, because I created them using a Sheet metal part.

    •    Your saved settings can be predefined per model type and model size (for assemblies) on the Drawing View Wizard tab (Solid Edge Options dialog box).

     

     

     

        Items stored in the saved settings:
    o    All properties from the properties tab.
    o    View orientations
    o    Custom orientations
    o    Best Fit
    o    Set View Scale
    o    Shading Options
    o    Edge Colors

    •    Saved Settings file will be created in the reports directory called DraftWizard.txt.

    Once you’ve created a list of saved settings, I believe that you’ll find the new approach more efficient and easier to use. But if you still prefer the old method, you can still use it. As always, if you have any questions, and are a customer of ours, please call us on the toll free tech line at 1-877-215-1883 or email us at support@designfusion.com. If you are not a customer of ours, please contact your reseller for further support.