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Designfusion Blog

How to video: Frame Design

Manny Marquez - Tuesday, September 02, 2014
Check out our latest Solid Edge tutorial by Manny Marquez.


For more videos take a look at the Designfusion youtube channel here

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.

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/.

    Working With Revision Manager

    Manny Marquez - Thursday, January 09, 2014

    In the past few days, customers have called about revision manager and have asked several questions on how  they can move or copy assemblies to new locations.

    There were a few main issues custumers have had in regards to Revision Manager, and what I have done is created multiple scenarios to tackle these issues .  

     

    Scenario 1: Copy all assemly with all parts to new location.  

    Scenario 2: Copy all parts associated to assembly and folder structure to new location folder.

    Scenario 3: If a folder with parts related to an assembly gets nenamed  and links get broken, how to redifine links.  

     

    Sample Folder structure (this can be any combination of folder locations) the point is that, we need to move or copy files to a new location.    

     

     

              Scenerio 1: copy all assembly with all parts to new location, this is ideal when you need to clone

              the whole asssembly to send to a customer.  

     

    1. 1. Open TOP level assembly with Revision Manager.

     

     
    1. 2. Expand then select all, this option makes sure that all files will be copied. Notice action is unchanaged.

     

    3. Copy; this indicates the coping process.




    4.The next step is to set the path for the new location to copy the whole assembly.

     

     

     

    5. Final step is to perform actions. At this point the assembly is copied to the (new) folder location.
        However notice the subfolders are NOT copied.  This completes this scenerio.

     

     

       

              Scenerio 2:  Move the whole assembly with subfolder structure and related files only.

              Another method is just to copy all folders to the new location, but note that there may be

              files that do not relate to the assembly.

              In cases where you only need to move  files that relate to that top level assembly and keep the 

              same folder structure, files not related will not copy or move.  

     

    6. Open selected assembly with revision manager.

     

     

     

    7. We are going to move to (new location) and copy the same folder structure. By selecting the (rename)

        you are moving the files from the (original) folder.

     

     

     

    8. Notice action is to rename document.

     

     

     

    9. Now click on replace old folder (Original) with new folder (New). Then select replace all then cancel.

     

     

     

     

    10.Once replaced, see new folder with new location.

     

     

     

    11.Click on Yes and close Revision Manger.

     

    12.Notice the new folder structure in new location, notice the subfolders are copied as well.

     

     

     

    13.Review new folders using window explorer to take a look at the previous folder location; notice only

         files that were not associated to the assembly did not copy (This is also a good way to isolate

         assemblies) with the folder structure. This complete this scenerio.

     

     

              Scenario 3: Cases when a folder gets renamed and then you open the assembly and notice that

              all links are broken. This is very common in networks with many users.

     

    14.So let’s go ahead and rename each folder as shown below, just by adding “1” at the end of each

         word.

     

     

     

         If you try to open the assembly now with RM or Solid Edge, the files will not open; you will get a notice

         that files are missing.

     

     

     

    15.Click on the redefine links then select top level folder then ADD (make sure that the subfolder is

         unchecked).

     

     

     

    16.The easiest way to get the folder address correctly is by going to the window explorer, and then copy      and paste.

         -(ManufacturedParts) is the original folder

         -(ManufacturedParts1) is renamed folder

         -click next twice

     

     

     

    17. Click on Back twice  

     

     

     

    18. Repeat for other folders

     

    19.Next twice

     


        Close Revision Manager, and then reopen with top level assembly. This completes this scenario.

     

        This was also presented at one of our Solid Edge Productivity summits by Barry

        Shillingford.



    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.

    Setting up your CAM Express role in NX9

    John Pearson - Thursday, November 07, 2013
    Due to the increasing popularity of CAM Express, we are receiving more calls on our support line. The most recent calls have been requesting help in setting up the new NX9 CAM Express role and setup pallets. So to help those of you who will be making the switch soon, I thought I’d be pro-active and add these answers to our blog site.

    How do I set the CAM Express role in NX9?

    1. Open up the NX9 gateway, and click on the Roles tab.



    2. From the Roles pallet, select the CAM Express role.



    3. Click OK to the Load Role message.



    4. Open a Solid Edge part file or NX part file.



    5. Click on the Web Browser tab.



    6. Start your first setup from the Web Browser pallet, by clicking on the “Create a new setup for this model” shortcut, near the bottom of the pallet.



    7. Select the desired Units and then select the desired Setup, from the Create New Setup dialog. For example, below I selected Millimeters and the Machinery (Express) Setup.



    8. Click OK, to launch the selected setup.

    How do I turn on the Express Setup pallet?

    Once you have entered into manufacturing, using the previous steps, you can turn on your manufacturing pallets. 

    Notice the Manufacturing – Express tab is missing.



    1. Go to File > Preferences > Manufacturing.



    2. Select the Add Setup Pallet icon, under the User Interface tab.



    3. From the pallet list, select Express and click OK.



    4. Click OK to dismiss the Manufacturing Preferences dialog

    Notice that the Manufacturing – Express tab is now present.



    5. Click on the Manufacturing – Express tab and you now have access to all your Express Setups for future jobs.



    If you would like to learn more about NX CAM Express, feel free to contact us at info@designfusion.com. If you are a Designfusion customer, you can contact us at support@designfusion.com or call our support line at 1-877-215-1883.

    Ordered vs. Synchronous – Which should I use? – Part 2

    John Pearson - Thursday, October 17, 2013
    If you read Part 1 of this article, you’ll recall that I discussed the Pros and Cons of ordered and synchronous modeling. I also suggested that you should use both paradigms in an integrated approach to get the best of both methods. In this article I want to take a closer look at why some users claim that they can’t use synchronous modeling. There are some myths that are cropping up about synchronous which are simply not true.  Of these myths, the most prominent one is the following:

    I have complete control of my design in ordered, but not in synchronous.”

    This is simply not true. First let’s look at the first part of the statement. The designer only has complete control of the sketch if it is fully constrained. Plus that control is per sketch, there is no guarantee that changing that sketch will not negatively impact other sketches in the model. It takes a lot of work to constrain and relate all your sketches to get models to always behave in a set manner. For this reason many users don’t bother to put in the effort. Plus, if your company follows standard PLM practices, once you complete and review the model, it is released. A released model should never be changed anyway. You should create a revision of a released model to be able to update or modify it. If you don’t use released models, your perceived control of the model is only good assuming no one goes into your sketch and starts deleting your constraints.

    The second part of this statement is also false. Not only can you control a synchronous model, but you actually have more tools to do so. The main reason users go into the sketch is to change the dimensions. In synchronous modeling, driving dimensions are placed directly on the model, allowing the user easy access with the same dimensional edit control as ordered. Geometric relationships can be maintained by using the Live Rules, without first having to place any geometric constraints, or by locking down 3D geometric relationships. If you compare the 2D geometric sketch relationship to the 3D face relationships, you will note that they are almost identical.


    So the reality is that you can have complete control of your models in the synchronous paradigm. In fact you have complete control without having to fully constrain your sketches. Remember, the sketch is merely a launch point for the model; it does not drive the model. For those of you who have struggled to fully constrain sketches, you can appreciate how much time this will save.

    This statement brings up another issue with ordered modeling. Many users lock there models down to try and ensure easy edits in the future. The problem here is that you have to try and predict what kind of changes can occur, if any, in the future. So the user invests a lot of time locking down or constraining a model, that may never change, or may change in a completely different way than the user predicted. If the model does change in the predicted manner, the designer still has to remember how it was originally constrained, in order to make predictable edits. The reality is that some parts never get changed, and those that do, are often changed in an unpredicted manner or, by a different designer. Even if it’s the same designer, he/she may not remember how it was originally constrained. Thus you spend more time trying to understand how the model behaves, even before you can attempt any edits.

    This doesn’t even take into account the parts that are often grabbed to use as reference parts. It’s been my experience that most designers prefer not to start from scratch unless forced to. They will often look for similar designs from their legacy data, copy and rename the model, and then edit the model to meet the new criteria. This can sometimes prove to be a frustrating experience if the reference model is constrained differently than your new model should be.

    This is the beauty of synchronous technology. You do not have to predict the design intent at the time of creation. It enables you to determine the design intent each time you make a change or edit to the model. Let me give you a simple example of this:

    Below is a fully constrained sketch that I use in my fundamentals course.


    Notice that this has been constrained such that the circles for the holes are centered on the rounded top corners and will move outward symmetrically, if I increase the value of 3.000. Likewise the holes and rounds will move upwards if I increase the value of 2.000. All the walls are locked to either vertical or horizontal positions, and the center half circle’s radius is controlled independently.

    This sketch is used to create the base feature of the following model.


    Based on my design intent, I have predicted that the model could change in one of the following ways:



    I could also change the diameters of the holes and the radii of the rounds or center cutout.

    However, what happens if I need to make different changes that were not predicted or I use the model for a reference part to make the following models:

    All three changes above would require some editing of the sketch beyound simple dimensional edits. Making the same model in synchronous, I create the following sketch:


    Notice that I don’t show any geometric handles. I can use them, if they speed up the creation of the sketch, but I don’t need to pit them in. I generate the model using similar commands that I used in the ordered paradigm.

    Editing the model is easily done in one step, using the steering wheel and Live Rules. Not only can I make the predicted changes to the model:



    Note: Live Rules automatically maintains the concentric relationships between the holes and the rounds.

    But I can just as easily make the unpredicted changes to the model, by turning off the concentric Live Rule.






    Plus I could make many more modifications directly to the model. I could lock down the 3D relationships thus restricting my model as I did in the ordered paradigm, but despite protests from ordered users, this isn’t absolutely necessary. If you choose to lock all your geometric relationships, they will appear in the Pathfinder, under a relationship header.

    Even if I lock the model down, these locked relationships can be deleted from the Pathfinder, keeping it easy to edit. But keep in mind that you do not have to do this, because Live Rules will maintain those relationships without having to previously define them.

    Another big reason for not using synchronous is, as I noted in the Part 1 of this article, there are some limitations to certain features. Some users believe that any limitations justifies not using the synchronous paradigm. Again these users have not been fully trained and do not understand the power of integrated modeling. For example, synchronous modeling does not support dangling bends in sheet metal. This prevents user from creating contoured flanges along a curved edge. In the model below I created this using an integrated approach.



    Notice that the model was started in the synchronous paradigm and the contour flange was added in the ordered paradigm. If I edit the synchronous features, the ordered features are automatically updated. For example, if I move the one side of the part, effectively changing the overall width, the ordered contour flange updates with the symmetrical move.



    So I still have the benefits of synchronous editing, yet the ordered feature provides me with the feature currently lacking in the synchronous paradigm. In other words, I get the best of both paradigms. Any limitations in synchronous are easily overcome by using the integrated approach.

    Finally, and I know you’ve already heard this from me in several posts, make sure you attend training. Synchronous technology requires a good basic understanding before you see the true benefits. It has been described as a mind shift similar to that of transitioning from 2D to 3D. Most resellers offer synchronous training for experienced Solid Edge users. At Designfusion we have a 3 day synchronous course with an optional 4TH day for sheet metal.

    Another way of looking at this would be to ask yourself what you would pay for a new CAD system that will significantly improve your efficiency, thus saving you time and money. Now, if you are a current user of Solid Edge, consider that you already own this and the only thing stopping you from reaping all the benefits is 3 or 4 days of training.

    If you are interested in seeing how synchronous can benefit your company, contact your local reseller for a demonstration. If you are already a Designfusion customer, or would like to be, contact us directly at sales@designfusion.com or contact your local account manager. Synchronous technology is here to stay and will continue to get better. The sooner you learn how to use it, the sooner your will reap the benefits.