North America's Leading Siemens PLM Partner

Designfusion Blog

Solid Edge: A baker’s dozen of Tips and Tricks (Part 3 of 3)

John Pearson - Friday, August 07, 2015


  • 9.Configurations for draft

Much like you create a configuration for your exploded view, you can create configurations for later use in your draft views. To do this you need to first turn off all the components that you wish to exclude from the view. Then create a new configuration of the components you want to show in the draft view. To do this, select the configuration command:



Click on the New button.



Enter in the name of this new configuration.



You can later place this named configuration as a separate view onto a draft sheet.


  • 10.Placing configurations in Draft

When placing an assembly into a draft sheet, using the Drawing View Wizard, you can select from a list of configurations or zones.



Only the components in that configuration will be visible in the draft view.


Note:If you wish to create a parts list of this configuration, you can set the Part List to only show the configuration components. To do this, open the properties of the Parts List and go to the List Control tab. Notice the Configuration option half way down the right side. Expand this and select the desired configuration.



  • 11.Placing section views in Draft

To place an assembly section view into a draft view, you must first place the assembly into the view. You then right click on to view and go to the view properties. On the Section tab you will find a list of all the assembly section views. Simply select the desired section view and then update the views to convert the assembly view into the section view.



  • 12.Drawing View Depth

By specifying a drawing view display depth for a back clipping plane, you can simplify any type of drawing view so that geometry behind the plane is removed from the view. This feature can be used, for example, to reduce the visible clutter behind a section view or a broken-out section view.


The Set Drawing View Depth command is found on the shortcut menu when you RMB click on the view.



You can type in a back clipping plane depth or use the companion view to set a depth.



You can remove the drawing view depth by using the Remove defined Depth command on the shortcut menu.


  • 13.Dimension Automatic Arrangement


Use the Arrange Dimensions command to automatically group, select, and arrange linear dimensions so they don’t overlap drawing view geometry and annotations.



There are three different ways to arrange dimensions;

  • I.Select a dimension



  • II.Fence select – drag a fence around the dimensions



  • III.Select a drawing view will select all dimensions for that view.



Note:This automatic arrangement command now makes it easy for you to use the Retrieve Dimensions command and quickly arrange the retrieved dimensions.

Thus ends our baker’s dozen tips and tricks. If all or most of these are new to you, consider upgrading your skills by attending one of our training courses. Here’s the link to the standard courses we offer; We can also arrange custom training to meet your company’s needs. For more information contact your Account Rep or contact us at


NX Draft Feature

Stephen Rose - Wednesday, July 29, 2015


Most users are familiar with the need to draft walls of parts or tooling to a certain angle. For those that are not familiar: It is used in manufacturing to allow de-mold of plastic parts and castings, a design requirement of some sort of functional fit, or so that the cutter and possibly the holder have clearance when machining down in deep-draw cavities.


The NX Draft Feature command has different sub-types when applying draft angle to a model.In this example we will use the two simplest types From Edges and Tangent to Faces types.


Where to find it


The Draft Feature can be found several ways.If you are familiar with the traditional NX menu you will easily find it under Menu->Insert->Detail Featureà->Draft


If you are more comfortable with the NX Ribbon style interface you will find it in HOME->Feature Group->Draft


There is always the command finder where you can search the Draft feature and access it directly.


Here we have an unfinished (yellow) part with vertical side walls as our starting body.First we want to add a simple draft angle to the side walls.



We access the Draft Feature command, either from the Menu or the Ribbon Bar interface.



Ribbon Interface



Once in the Draft Feature:


1. We select Type of Draft from the drop-down list and pick From Edges.


2.We define the Draw Direction, in this case the Z axis.


3.We proceed to select the bottom periphery edge of the part.


4.We set the angle to 5° and then with the preview option turned on we see the model updates to having 5° draft around the entire edge.(NX is smart enough adjust the upper radii

without the need to remove the radii and reapply after the draft command.)We use OK to apply this draft and exit the dialog box.



With the body drafted we now want to add a Hole Feature.In this example we set the Counter Bore Diameter large enough, and the position of the hole far enough over, so that the Counter Bore breaks out the side of our body.



With the C’bore subtracted the resultant part shows that there would be sharp material conditions where the holes break out the side of the body walls.(Note: In this picture we have also mirrored over the feature for better clarity of the conditions)



We want to clean up this condition by straightening the C’bore surface so they end up breaking out 90° to the side walls.



We enter the Draft Feature once again:


1. We select Type of Draft from the drop-down list and pick Tangent to Faces.


2.We define the Draw Direction, in this case the axis must point away from the concavity of the c’bore-Y axis (not into it as +Y) as indicated by the orange arrow .



3. We then select the C’bore face that is to be drafted.



4.We set the angle to 0° and then with the preview option turned on we see the model update to having 0° draft to the axis, but starting tangent to the C’bore face.




After hitting OK to accept the draft we end up with the modified part body as shown.(Note: In this picture we have also mirrored over the feature for better clarity of the conditions)




This type of modification can be very useful in part/product design to clean up features and eliminate sharp corners in a mold. It can also can play a part in the tooling industry by opening up areas for milling machines. Opening up various break out areas on tooling can increase the amount of machining strategies available to complete a particular feature.In this case access to the side of the feature is now possible.Efficiency could be realized by allowing use of profile or other machining methods to complete the majority of this part, rather than having to mill down the vertical axis of the feature only.



If you would like to learn more about this operation and other advanced operations, you should attend one of our advanced NX CAD courses. To arrange for advanced training please contact your Account Manager, or contact us directly at

Solid Edge: A baker’s dozen of Tips and Tricks (Part 2 of 3)

John Pearson - Tuesday, July 21, 2015


  • 5.Direct editing tool in the ordered paradigm.

The direct editing commands in Solid Edge allow you to modify models imported from other applications that do not have a feature tree, or to modify native Solid Edge design models without accessing the current feature tree.




Notice that in the Move Faces, Offset faces, and Rotate Faces, there is a select option to select the body.




This allows you to move, offset, or rotate the entire body.

  • 6.Flash Fit, for bolts and screws

When using the FlashFit option to place assembly relationships, you can select the bottom cylindrical edge of the bolt head and the top cylindrical edge of the hole to fully position the fastener, like the insert relationship.




Resultant relationships are Mate and Axial Align with rotation locked.



Note: To select the cylindrical edges you have to have the Circular Edges option turned on in the Assembly Relationship options.




  • 7.Capture Fit

Ideal for hardware or commonly used components, capture fit remembers what relationships and geometry you used to originally place your component. When you place the component again it will prompt you only for the target geometry.


To use capture fit you must first place the component into an assembly using the assembly relationships that you plan to capture. Then select the Capture Fit command and save the relationships in the dialog.




  • 8.Section views in assemblies

In the assembly environment, the Section command is found on the PMI tab.




The steps are similar to constructing a cutout feature for a part.


•Plane Step

•Draw Profile Step

•Side Step

•Extent Step

•Select Parts Step


For the last step you have options on how to determine which parts are to be sectioned.




When you are finished, you are left with a visual section view.




Note:You can hide and show the section view by toggling it on and off in the PathFinder.



Solid Edge: A baker’s dozen of Tips and Tricks (Part 1 of 3)

John Pearson - Thursday, July 02, 2015


Recently Designfusion held their annual Productivity Summit at the Microsoft office, in Mississauga. As part of the summit I presented a “Tips and Tricks” session that was well received. I promised that I would share these in a future blog article. So here is a baker’s dozen of tips and tricks:

    • 1.Holding down the Shift Key when using the Rectangle by Center command will create a square. (Added in ST7)




  • 2.Auto dimensioning done the correct way.

The biggest complaint with auto dimensioning is “I have to delete more dimensions than I would normally place”. However, if you use these settings Solid Edge will only place keyed in dimensions.


  • 3.Controlling rotation point
  • In the Select mode, Middle Mouse Button (MMB) click, in an empty screen space, to clear the small white select symbol attached to the cursor. The cursor will now appear with no symbols attached.




  • Move the cursor to one of the following positions and hold down the MMB to rotate:
  • I.Hold the MMB down on a vertex to rotate about the vertex.




  • II.Hold the MMB down on a linear edge to rotate about the linear edge.




  • III.Hold the MMB down on a face to rotate about the point on a face.




  • IV.Hold the MMB down on a circular arc or conic-shaped edge to rotate about the axis of the circular arc or conic-shaped edge.




  • 4.Clipping planes

I.Choose View tab→Clip group→Set Planes.




II.Select a planar face or reference plane, position the cursor to define the first clipping plane (A), and then click.

III.Position the cursor to define the second clipping plane (B), and then click.




IV.Click Finish.




Note: When you set the Dynamic Clipping option on the command bar, the clipping depth updates dynamically as you move the cursor during the Set Plane 2 Step. When you clear the Dynamic Clipping option the clipping depth updates when you click to define the second clipping plane.

Note: You can turn the clipped display on and off using the ‘Clipping On’ command, located below the Set Planes command, or use the Hot Keys (Ctrl + D).



Transfer of loads from Motion analysis to FEA study within Solid Edge

Frederic Menage - Thursday, June 11, 2015



Check out our other videos :

How to: Dimensions in Draft Part 3

Manny Marquez - Thursday, June 04, 2015

Part 1:

Part 2:

More videos here:

Using a Contour Surface Area operation to do undercutting

John Pearson - Thursday, May 21, 2015

Recently I had a customer contact me with a part that he wished to undercut. He needed to use a spherical cutter, which eliminated the Groove Milling operation, since it only uses T-cutters. Not being an advanced user he was unsure how to proceed. With his company’s permission I’ve decided to utilize this opportunity and create a blog article on how to use the Contour Surface Area operation to do undercutting.

Below is the image of the part along with the faces (highlighted in orange) that need to be machined.




Before creating the operation I need to generate some geometry to use as Drive and Projection geometry. First I create a small cylinder, protruded through the center of the part (shown below in magenta). This cylinder will be used for my drive geometry. In other words, I will initially create my tool paths on the cylinder and then project them onto the surface of the part.



I place this cylinder on an unused layer so I can easily hide and show it as needed. Next I create a line along the axis of the cylinder (shown below in yellow).



I place this line on an unused layer so I can easily hide and show it as needed. I will use this line to help project the paths from the drive geometry onto the surface of the part.


I then create my parent groups. For the Geometry group, the customer had created a WORKPIECE1 that contained the part and was a child to the MCS shown below. He’d also created the spherical mill for the Tool group, also shown below.




Along with the predefined PROGRAM and MILL_FINISH method I now have enough information to begin the operation.


I select the Contour Surface Area operation and assign the parent groups as shown below.



Once in the operation, my first step is to specify the cut area.



I click on the Specify Cut Area icon and select the faces that I wish to machine, as shown below.



Next I need to define the Drive Geometry. I select the Edit icon (small wrench) in the Drive Method section.



I then select the Specify Drive Geometry icon.



I turn on the layer that contains the previously created cylinder. Select the cylinder as shown below. Remember the surface will be used to create my initial tool paths.



I click OK to return to the Dive Method dialog. I then expand this dialog and set the drive settings and tolerances as required by the customer.



I can verify the results, of my drive geometry settings, by clicking the Display icon under the Preview heading. Notice the orange surface mesh representing my drive geometry.



Once I have my drive geometry created, I return to the main operation dialog to select my projection vector. To do this I first turn off the cylinder layer and turn on the line layer previously created. I then set the Projection Vector to Away from Line, as shown below.



I’m prompted to specify the Line/Vector, so I select the line that I had previously created. By doing this I’m telling the system to project the tool paths on the cylinder away from the axis towards the surface of the part.



Next I ensure that my Tool Axis is set to +ZM Axis.



I then modify the Engage motion, to use the center point of the opening, as shown below. This ensures that any engage motion will start in the center of the part.



I then set my Retract motion to match the Engage motion.



Finally I set my feeds and speeds to the required values, and then generate the operation. Notice the resulting undercut.




The Contour Surface Area operation allowed me to define how I was going to machine the cut area, by defining a cylindrical drive surface and projecting it away from an axial line, onto the cut area.


If you would like to learn more about this operation and other advanced operations, you should attend one of our advanced NX CAM courses. To arrange for advanced training please contact your Account Manager, or contact us at  


​How to build a study with many connected parts

Frederic Menage - Saturday, April 25, 2015

 (Assembly environment – Simulation module)


When there are many parts in a study, the amount of connectors (created automatically or manually) can be overwhelming. I t is important to remain in control of those connectors as their quantity increases. Otherwise, it will be a difficult task to find the source of the problem when a fatal error occurs during solving.


A recommended method for medium size assemblies

The user of Solid Edge can include only a subset of the parts that will eventually need to be analyzed. This way, a limited amount of connectors will have to be created. The workflow is to modify the boundary conditions to accommodate this partial study (add temporary load or constraint) and solve to verify that the connectors play their role and keep the studied parts connected. Then, the user can modify the definition of the study to add more parts or start from a copy of the study to keep a backup of each step. Each following steps, necessary to build the full study, will require the addition of new connectors and modification of the boundary conditions.


A recommended method for large size assemblies (with thin walled parts)

The user of Solid Edge should use mid-surfaces (psm) or other type of surfaces when analysing thin-walled parts. In addition to this, the user has the option to connect surfaces and create one or several associated bodies for the analysis. This will remove the need for connectors as the nodes merge at the intersections. This approach needs to be considered seriously when hundreds of parts are being analyzed.


With these workflows, the Solid Edge user who wants to build a complex analysis can confidently and progressively add all the required simulation features to run a full study. The capacity to verify a subset of connectors and, afterwards, move on confidently to the next group of connectors can be a huge time saver when dealing with large assemblies.

How do you Change the Default Settings in the Operation Templates

John Pearson - Wednesday, April 22, 2015

 Manufacturing software has come a long way over the years, and it continues to improve as the machines and hardware evolve. However, the software may not be designed to handle your specific task. It is often necessary to modify settings in the operations to meet your specific needs. For example you may have to modify the cut pattern, the step over distance, cut depths, speeds and feeds, etc. If you find yourself constantly modifying settings, you may want to look at customizing your CAM software.

If your software is NX CAM Express, you can customize the package using several tools. The nice thing about these tools is that you do not have to be a code writer to use them. NX allows you to customize your CAM package in the following ways:

  • 1.Customer Defaults For Manufacturing

2.Manufacturing Templates

3.Definitions of Output formats

4.Definitions of libraries and library data

5.Process Assistants


Further details on these topics can be found in the NX CAM help documents, but for this blog article I’d like to focus on one of the more common requests, that I get on our tech line. How do you change the defaults settings in the operation templates? Believe it or not this is one of the easier things to do in NX CAM. However it does require some knowledge of the inner workings of NX CAM Express.

NX CAM Express Setups


Normally you start your manufacturing program by launching one of the pre-defined setup programs. For example, you may select the Machinery Express setup in Metric.




This opens the manufacturing environment, creates a manufacturing assembly and loads the Machinery Express operation templates. It knows what operation templates to load from this file:


C:\Program Files\Siemens\NX 9.0\MACH\resource\template_dir\template.dat

If you open this file in NotePAD, and view the list, you will see the line for the Metric Machinery Express setup.




The rest of the line lists the operation templates part files which NX will load for this setup.




The metric part files are stored in the following location:


C:\Program Files\Siemens\NX 9.0\MACH\resource\template_part\metric\

If you wish to change the defaults in the operations templates, these are the files you must edit.

Note: NX 9 added a new folder for updates. This folder contains the updated copies of the operation templates when you install a QRM or patch. The folder is:

C:\Program Files\Siemens\NX 9.0\MACH\updates\template_part\metric

The option to ignore this updated file is found in the Customer Defaults, under Manufacturing - General. If toggled off the original files are loaded.


Changing the defaults

So now that we know where the operation template files are saved, how do we edit them? Referring back to the template.dat file we see that the name of the file we need to open is the Machinery_Exp.prt. So we open the Machinery_Exp.prt found in the C:\Program Files\Siemens\NX 9.0\MACH\resource\template_part\metric\ folder.


Notice the Operation Navigator of this file lists all the operation templates that we can choose from when we attempt to create an operation under this setup.




Lets assume that we want to change the cavity mill default Stepover from a 50% to 75%, of the tool flat. To do this we open the CAVITY_MILL operation and change the Percent of Flat Diameter to 75, as shown below:




Click OK to close the operation. Now you must save the change. However this is most likely a “Read-Only” file, and even if it’s not, it’s a good idea to keep the original file. Therefore I recommend that you save it as a unique file. For example, I save mine as DF_Machinery_Exp.prt (DF for DesignFusion, in case you’re wondering).


Next I have to tell the system to load this new file when I launch the Machinery Express setup. So I open the previously mentioned Template.dat file and modify the name of the file to match my new name, as shown below.




I then save and close this file.


Testing the new settings

To test that the new default setting is working, open a new part. Run the Machinery Express setup in Metric.




Create a new cavity mill operation.




If you’ve done it correctly, you should see the new default value appear, as shown below.




Keep in mind that it’s always good to keep a back-up of the original files and your modified files.


I know that editing installed files can be intimidating to some users. For this reason, Designfusion offers customization services. If you’d like us to provide this service for your company, please contact your Account Manager, or contact us at     

How to: Manage Dimensions in Draft Part 2

Manny Marquez - Thursday, April 16, 2015


Part 1: