Posts Tagged ‘Sheet Metal’


Integrated Modeling in Solid Edge

Monday, November 19th, 2012copyright

With any new technology, you have your early adopters. This is followed by a general acceptance of the new technology, and of course, you always have your hold outs or late adopters.  Solid Edge ST and ST2 appealed to the earlier adopters for synchronous technology. With ST3, ST4 and now ST5, we are seeing most of our customers starting to use synchronous modeling. This of course has led to many questions. The most asked question is; “Should I use synchronous or ordered modeling?” The answer to this is yes.

One of the unique qualities of Solid Edge is that you are not locked into using synchronous or ordered modeling. Integrated modeling allows you to use both synchronous features and ordered features within the same part or sheet metal model. As a rule of thumb, I encourage users to start with synchronous modeling. If they run into some issues that can’t be addressed with synchronous features, they can switch to the ordered paradigm to complete
the model. Let me illustrate this with the following example:

I wish to model the sheet metal cover shown in the following image.

I start in the synchronous paradigm and create a tab, for the top of the cover.

I then add 2 synchronous flanges, in one step, to create the back and left side of the cover.

One of the current limitations, in synchronous sheet metal modeling, is that you cannot drive a flange along a circular edge. Realizing this I will hold off creating the front and right sides until the end, when I will use an ordered feature.

I next use 2 bead synchronous features to create the slots at the top of the part.

I then transition to the ordered paradigm to complete the model.

I use the ordered Contour Flange command to create the front and right face of the cover.

The nice thing about this approach is that it still allows me to modify the model using the synchronous Move/Rotate command.

Live Rules and all the other synchronous editing tools still apply to the model.

As I modify the model, synchronous features update instantly, followed by the re-computing of any ordered features.

For those of you who attended our productivity seminars, you saw this demonstrated live. Other users have learned this process in one of our many synchronous modeling courses, offered over the last year.

This is just one of many examples where Integrated Modeling allows you to benefit from the new synchronous technology, while still utilizing some of the tried and true methods of the ordered technology.  As Solid Edge continues to develop the synchronous features, you may find that you’ll use less integrated modeling. But for now this provides you with a reliable and safe platform to further advance your adoption of this amazing new modeling paradigm we call synchronous technology.

If you’d like to learn more about integrated modeling, you can attend one of our synchronous modeling courses. For more information visit our website at New 2013 courses will be added to our schedule soon.


Editing Part/SM Operations in Assembly

Monday, November 5th, 2012
In ST5 you can now perform edit operations, from the assembly environment, without first in-place-activating to enter the model directly.  Things you can do:
  • Locate, select and edit of ordered features
  • Edit synchronous procedural features
  • Delete synchronous face-sets and ordered features
  • Move face-sets (sync feature) in synchronous parts
Let’s take a look!
Firstly, ordered features are now selectable via the Face Priority select option. (remember hotkey combo is CTL + Spacebar)
Notice in the example below that “Protrusion 1” is available from the Quickpick options in assembly now.
Once selected, “Protrusion 1” has its options displayed for going directly into the features parameters.
Select whatever you would like to edit and SE will take you directly there.  Once complete, just close and return.  This will take you back to where you were in the assembly.
This saves time from previous versions by allowing you to go directly to what you want to modify and brings you back to the assembly reducing the number of mouse clicks.
Editing synchronous procedural features from the assembly level does not in-place-activate the user into the part.  Procedural features are things such as Patterns, Thin wall, Helix, Hem, Dimple, Louver, Drawn cutout, Bead, Gusset, and Etch.  These are editable directly in the assembly.
Using Face Select again, “Louver 1” is selected.
The handle for the procedural features shows up.  If selected we are presented with the following options.
Also, if we were to select the adjacent lover we would be presented with the following options:
Notice that the option to edit the pattern is there.  I know what the usual next question would be “How would I know how to edit the parent of the pattern?”.  Notice the option for “Louver 14”.  If you were to select it, you would be presented with the same options as previously mentioned.
We select “Pattern 1” and now we can modify the parameters that define the pattern.
Once selected, click on the PMI callout “Pattern 2 x 4” and we will get the following options:
Notice we have not left the Assembly environment.
One thing to note about this type of editing: Procedural Feature profile editing requires in-place-activating first.  Also, there is no access to the profile handle from within the assembly.
Happy Edging!
If you would like to learn more about “What’s New in ST5”, stay tuned for our new Update Training course.  For information related to training from Designfusion follow this link: ( conditions
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Accelerate tool design with a few simple surfacing commands

Friday, September 14th, 2012

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

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

I will insert this as a construction body.

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

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

I select all the inner faces of the dimple.

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

Next I create a symmetric protrusion which encompasses the surface.

I then select the Boolean command.

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

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

The protrusion is trimmed from the surface, as shown.

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

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

Many users are unaware of the powerful surfacing commands in Solid Edge. As shown above, these simple yet powerful commands can significantly accelerate your design process. If you would like to learn more about surfacing, we offer training in our advanced modeling class ( or you could try the self-paced training course online at


Etching in Solid Edge

Tuesday, November 15th, 2011copyright

Engraving or scribing with a laser machine can be achieved with the Solid Edge Etch command. The Etch command is supported in both the Ordered and Synchronous sheet metal modes. It is available in both the folded model and in the Flat pattern.


A Sketch must exist in the model for the command to be active. Remember text can be entered into a sketch with the Text Profile command. (See a previous entry, on our blog at


Creating an Etch

Once you have created the sketch the Etch command becomes active.


 The Etch command allows the user to select single or chained sketches


Note:  With the single option selected, multiple sketches may be selected with a fence selection, if they are part of the same merged sketch.

Etch options are provided to allow the user to control for colour, line width and line type.


Note:  Etches can be created in the folded model state or in the flat pattern state. If the etch is created in the folded state it will transform position with the Flat pattern. Etches created in the flat pattern only exist in the Flat Pattern node and do not exist in the folded model.


Editing an Etch

Ordered etches can be edited using the standard edit, edit profile, or dynamic edit commands.


Synchronous etches are procedural features. When you select the feature an edit handle appears.


When you click on the edit handle the Feature Origin appears. This allows you to move or rotate the etch using the steering wheel. The Edit Profile handle also appears allowing you to edit the etch profile.


Note:  PMI (3D dimensions) can be placed to the Etch feature, or to the Etch feature origin, to drive or lock the features position.

In the edit mode, the user can specify a new layer face to which to apply the Etch.

Note:  Etches cannot span across bends or multiple layer faces.

Etches in Draft

The Etch features in Draft are treated as a construction object and are listed in the Construction section of the Drawing View properties.

Etches are automatically displayed by default.

Exporting to DXF

Options have been added to the Save as Flat command allowing you to export the etch feature to a .dxf file and also to control how it is exported to a .dxf file.