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Using IFC files with Solid Edge ST8

Francis Robert - Tuesday, February 02, 2016

Solid Edge ST8 can now import and export « IFC » files. This “Industry Foundation Classes” format is actually a neutral 3D file which allows sharing geometry and properties between a CAD tool and “BIM” applications (Building Information Modeling).We could compare an IFC file with a STEP file for example; difference is that the IFC format also contains a suite of properties used in the Construction and Architecture industries.The IFC format is developed by an international committee and is not owned by any CAD vendor in particular, therefore the “neutral” file nickname.


Solid Edge ST8 supports two types of IFC files, IFC2X3 and IFC4. The IFC2X3 type doesn’t contain precise geometry (Brep is NOT supported) and less properties.This type is closer to a STL or JT (without precise geometry) file.Whenever it’s possible, it’s better to use the later IFC4 type.It’s more recent, does support precise geometry (Brep) and can carry more properties.These properties are closely tied to the Construction industry, like electrical consumption for example.The application that reads the IFC4 type will be able to add the geometry to its general layout, automatically going on the correct Field / Building / Story, adding the electrical consumption to the overall building consumption, for example.Please note that you need to install Solid Edge ST8 Maintenance Pack 3 in order to manage these additional properties.

1. Simplification


We strongly suggest simplifying the geometry before exporting the model to the IFC format.While you can always export the model as is, your partners and customers will appreciate the fact you took some time to remove unnecessary details (hardware, internal components, etc.). When your product is positioned into a building, you can remove details without impact.By simplifying geometry, the global performance will be much better and you won’t share all the fabrication details (and intellectual properties) with your customers.


Solid Edge offers efficient simplification tools at the part level as well as at the assembly level. This allows you to remove faces not required in the final model (chamfers, fillets, internal details, etc.) while keeping a single file per part to maintain.


Solid Edge will export the IFC model in its « as displayed » state. So if non-required parts are displayed, you should hide them before exporting, check the correct option, and the IFC model will look exactly as you want to.Same thing applies to the “Design” or “Simplified” display state of parts.

2. Properties management


Before exporting to IFC format, you need to make sure the properties are defined correctly.This is the primary purpose of this format.If there were no benefit in sharing properties, you could simply use existing neutral 3D formats like STEP and Parasolid.


For type IFC2X3, the list of properties is limited to Author, Organization, Program and Description). We access these properties via the IFC export options.In Solid Edge, select Save As, then the IFC format and the Options button will become available.



Type IFC4 is more recent and can carry as many properties as desired.Again, in the IFC export options, you can select « Include IFC properties ».This enables the link to an Excel spreadsheet used to define properties groups, names, types and values.We can have as many spreadsheets as required.



The default XLSX file supplied with Solid Edge is located in the Program sub-folder of the ST8 installation folder. There are instructions in the first tab and a suite of properties given as an example.We suggest backing up this file and using it as your foundation to define your own list of properties.


Each of the following tabs is used as a property group. Each group contains a list of properties, each with their name, value and type.You can create and remove groups and properties to make sure to cover the needs of each of your projects.For multiple customers with different needs, we suggest to create a spreadsheet for each one of them.You’ll only need to select the appropriate spreadsheet when exporting your model.

  • Portions of the default XLSX file supplied with ST8 MP3:

  • For example, group « Pset(Common) » contains general properties for every basic IFC file. Another groupe like “COBie” (Construction Operations Information Exchange) corresponds to generic properties used in the Construction industry without regards to actual geometry.

3. Export


Once the model is simplified and the properties correctly defined, you just need to hit « Save ».You’ll see file size compression in the process, especially with the older IFC2X3 format.



Solid Edge ST8 can also import IFC files.You will probably see additional assembly levels than the model you exported. Since IFC format is aimed at Construction projects, it will add a couple of levels of sub-assemblies above the actual model.They correspond to Construction Site / Building / Story.This allows architects easier management of building components.


If you import an IFC2X3 type, you won’t be able to select the geometry in Solid Edge.This is because the geometry is faceted data, not precise geometry.You only have the « visual » portion; there is no « mathematical » portion (Brep).Therefore, the IFC2X3 usage is very limited when opened in a CAD tool but you can still use it as a reference. You will not be able to select a keypoint, create a draft, display visible edges or even do a boolean operation.This is similar to the usage of a STL or JT (without precise geometry) in Solid Edge.


If you import an IFC4 type, you will remove the limitations mentioned above. IFC4 contains the “Brep”, so there is precise geometry in the file.You’ll be able to use it as with any other imported CAD format, similar to a STEP or Parasolid.Even the parts’ colors will be imported.


As you see, we strongly suggest using the IFC4 type whenever you can.

5. Conclusion


With a couple of tries, you’ll be able to find the right balance in the level of details (what do you simplify?) and the list of properties to share with your customers and partners. You’ll be able to share your products intelligently with all architects on the planet in a complete and precise fashion.

How to Find the Volume Capacity of Container

John Pearson - Thursday, January 28, 2016

It is sometimes necessary to determine the volume of a container. This is a relatively easy process to do, if you understand a few simple surfacing commands. For this article I will use the Hopper pictured below.



In this example I need to know the volume of sand that this hopper can hold. To determine this, I need to create a construction volume of the inside of the assembly. For this to work efficiently I need to know that the assembly is assembled correctly. In other words, I don’t want any gaps between the seams or joints of the hopper. Once I’m sure that this is true, I use the Create in Place command to create a part within the assembly. I give the part a name like Volume1.prt. The command then places me inside the Volume1.prt with the underlying assembly components visible, but dimmed.



Next I use the Inter-Part Copy command and I get all the inner faces of each part in the assembly.



For example, the Inter-Part Copy command prompts me to pick a part to copy from, so I select the back part, as shown.



I’m then prompted to select what I want to copy. I set the selection filter to Face and select the inside face of the part.



I accept this selection and I am left with the inside face construction surface.



I then repeat these steps for all of the components in the assembly. Once completed, I hide the assembly components by using the Hide Previous Level command. This is found on the View tab, in the Show group. I am left with all the inside faces of the hopper.



Note: If your assembly components are aligned properly these faces can be capped and stitched into a solid. Poor alignment may leave gaps and require more work to stitch the surfaces together.


Next I will use the Bounded command, from the Surfacing tab, to create end caps on this surface model.



I select the four top edges to form a closed loop and accept them to create a flat surface at the top.



I then repeat this step to create a bounded surface on the bottom. Note, the order in which I create the surfaces is not important, but I must have all the surfaces created before proceeding to the next step.



To turn this into a solid, I will use the Stitched command, found on the Surfacing tab.



I accept the defaults when the Stitched Surface Options dialog appears and hit OK.



I select all the surfaces and click Preview.



If I have aligned my components, and extracted the correct surfaces, I should receive this message.



I hit OK, and I’m left with a solid body representing the inside of the hopper.



To find the volume, of this solid body, I go to the Inspect tab and click on the Physical Properties command.



When the dialog appears, I make sure to click on the Update button, at the bottom. Since I haven’t assigned a material, I get this warning message.



Since I don’t care about the mass of the solid, I hit OK and the system gives me the volume of the solid.



I now have the capacity volume of this hopper. I can save this part with the assembly, but have it not appear in the draft files, or bill of materials, by setting omission options in the occurrence properties.


If techniques shown in this blog are unknown to you, I suggest you attend some of our advanced courses. Surfacing is taught in the Advanced Modeling course and Physical Properties and occurrence properties are taught in the Advanced Assembly course. For more information visit our website at or contact us at [email protected].


The right tool for the right job (part 2)

Dominic Benoit - Tuesday, January 26, 2016

In the first part of the article “The right tool for the right job”, I started illustrating one of the aspects where the drawing and the programming software reach each other. In the following, I’ll point out some other elements that belong to each application type.


Once opened in the Drafter application of act/cut, the drawing can be modified, corrected and rotated by the user in order to match the horizontal orientation of the part with the horizontal direction of the plate. It’s particularly useful for the parts with brushed finish or that will be cut in a plate with a pattern. If it contains doubled or overlapped lines those will be eliminated and if the endpoints are not connected, it will become apparent.



Fig. 3- act/cut shows a red X where the contour is not closed.


For a subcontracting company who receives all sorts of drawings, it is essential to be able to make the necessary corrections to ensure manufacturability of the parts and avoid returning the drawings to the sender to offer faster delivery. The tools are in place in the Drafter of act/cut to repair typical imperfections.


For a continuous cutting technology, act/cut will determine a cutting direction according to the machining operation (left or right kerf compensation). To achieve this, the external contour of the piece must form a continuous chain. Solid Edge meanwhile provides no indication of the direction of the profile chain. This information is required especially for the continuous cutting technology.


On a counterpart, the Solid Edge user can determine the orientation of the flat pattern when he uses the Flatten command. Solid Edge will output a clean geometry, without doubled or overlapped lines nor disconnected junctions.


After orienting the part in act/cut, the programmer can decide to authorize the part to be rotated in the nest to improve part placement or prevent it from rotating to respect the grain direction of the sheet.



Fig. 4- Nesting authorization settings in act/cut.


For better cutting finish, some machine can adjust their speed based on the size of the contour to cut (diameter or perimeter), it means that each contour within a part will be using different cutting parameters. For that reason, the act/cut user must use auto-tool allocation to apply proper parameter to each contour.



Fig. 5- The colors indicate that act/cut recognized the machining parameters according to the size of the contours.


After the parts are all prepared, they will be regrouped per material/thickness in a Launching order in which one can specify the quantity of each part to produce and also the selection of sheet size available to nest. Following this, the optimal toolpath is generated and the nc program is being written for the complete nest.


As you may notice, whether in the drawing or in the programming software, a lot of tools exist to ensure a good integration of the various platforms with each their speciality. Should you be a manufacturer with your own cutting machine or you outsource the task, being aware of the parameters and the needs of each other’s platform will help streamline the exchange process.


The right tool for the right job (part 1)

Dominic Benoit - Tuesday, January 19, 2016

Often times we are being asked: “Can Solid Edge do the programming for the machine that is going to produce the parts? ” My answer always comes to the principle that every pieces of software has its speciality. For example, when it concerns sheet metal parts, it will be cut on a continuous cutting technology (Laser, plasma, milling) or on a punching machine. As we can assume, each type of machine has in strength. Some technologies are better for thick material while others are very fast on thin parts. Some have a large size stationary table; other like the punching machines have a moving table and other can only hold one piece at a time. Here I refer to wood panel machining center with a wide array of tool type (saws, drills, mills and even label printer) and can machine on several faces of a part. This quick overview is just illustrating the range of specialisation that is involved when we think of programming a part to produce.


Solid Edge is an engineering and drawing platform. Programming software is essential in the preparation (offline) of the programs that will run on the machine. Moreover, all machines don’t “speak” the exact same language, even though the G-Code format is standard, taking into account of the level of instruction that the machine manufacturer put in the head (the controller) of the machine. So, every time that a software writes a program for a specific machine, it has to know what instructions the machine is expecting, how it’s expecting it and also, which ones don’t need to be given. This task belongs to the post-processor that goes with the programming software.


At the drawing stand point, there is no way we can specify that much information precisely for the manufacturing technique. So, outputting the outer and inner contours of the geometry that need to be cut or engraved is enough. Another article on our blog explains how to use the command that prepares the drawing for manufacturing a sheet metal part (How to save a flat pattern as a .dxf file in Solid Edge).


Programming applications all have their level of comprehensiveness of the programming needs particularly if they are developed by a machine manufacturer or by an independent software editor.


The programming software that I’m talking about in my article is act/cut, edited by a French company Alma, it is independent of any machine manufacturer. Act/cut’s strength is in its ability to be adapted to communicate with various types of machines within the same environment and in its calculation algorithms for nesting parts.


The most common exchange format for manufacturing drawing is of course .dxf. That’s why it seems logic for Solid Edge to export in this type with the command Save as flat. It’s also logical for act/cut to import this format smoothly. Act/cut can also import native CAD files from well-known software thanks to an add-on module.


When a .dxf is opened of the Drafter application of act/cut, a filter can be used either by Layer, by color or both Layer/color. This filter allows eliminating undesired elements up-front. For example, 2D drawings often have some dimensions on a specific layer, we don’t want to cut those as part of the piece, and then we remove them right away.



Fig. 1- Layers filters in act/cut.


Some parameters can be setup in act/cut’s resources to indicate in advance which layer or color must be excluded or included and what type of contour are they representing. Does it represent geometry to cut or to engrave or even is construction or cosmetic? This leads to enable batch import of files.


For its part, Solid Edge also provides parameters to control layer filtering in the Save as flat command. Once set, these parameters are stored in order to prevent from having to redefine them again each time.



Fig. 2- Layer filters in Solid Edge.


Many other aspects are to be considered in determining what role is played by which software regarding parts fabrication. I’ll cover more in an upcoming article.


Moving or Renaming a Subassembly with Revision Manager

John Pearson - Friday, December 18, 2015

For those of you that use revision manager, this may be a non-issue, but some users still have an issue with intelligently moving or renaming subassemblies or parts. So at the risk of over simplifying the issue, I’ve put together a simple example to illustrate how to achieve this task.


The scenario: I have created a Test folder representing my server. Inside this folder there are 5 other folders as shown below:



Folder1, Folder2, and Folder3 each contain a different assembly. These 3 assemblies all use a subassembly that currently resides in the OLD folder. The goal is to move and rename the subassembly from the OLD folder to the New folder, without breaking the links to the 3 assemblies in Folder1, Folder2, and Folder3.


To start the process, I open the OLD folder, locate the subassembly, and RMB click on it to select “Open with Revision Manager”.



Note: I could also open the View and Markup program from the Start Programs menu and then open the file in Revision Manager, from View and Markup.




Once in Revision Manager, I highlight the subassembly and its components as shown below.



Note: If you click on the top left grey square, it will highlight all the occupied rows below it.



Next, I go to the Tools tab and select the Where Used command, in the Assistants group.



The Where Used dialog appears and allows me to set up my search scope. In this example, I want to search the TEST folder in my C drive. Notice that I have also toggled on the Include subfolders option, near the bottom of the dialog.



Note: Under the Process options button, I could filter the type of files that I am searching.


Once my search scope is set up, I click Next. The process runs and reports back to me the Number of documents processed: and the Number of documents found:



I click Finish, to dismiss the dialog. I am left with a list of where the subassembly and its components are used. Remember this list is only based on my search scope. If the subassembly or its components are used outside of my TEST folder, it will not show up unless I expand my search scope.



Now I will move and rename my subassembly. To do this I RMB click over the highlighted components and select Set Action to Rename.



Note: I could also click on the Rename command on the home tab, in the Action group.


Notice the New Filename column becomes populated.



I now either click on the Set Path command, on the Home tab > Action group, or RMB click and select Set Path from the shortcut menu. This launches a browse dialog. From there I select the New folder, which is the location that I want to move the subassembly and its components.



When I click OK, the New Filename column is updated to the new path.



Now I can rename the components. In this case, I want to replace the “exp” prefix with a “new: prefix. To do this I select the Replace command from the Home tab>Edit group.



I set the dialog up to find and replace “exp” with “new”, as shown below.



Once I completed this process I see the new names, along with the new location, listed in the New Filename column.



These changes have also occurred in the Where Used section of the Revision Manager.



Before I tell the system to make these changes, I need to tell it to update all the parent assemblies that use this subassembly and its components. To do this I first highlight all the listed parent assemblies, as shown below.



Next I either click on the Update command on the Home tab>Action group, or I RMB click and select Set Action to Update from the shortcut menu. This populates the New Filename column in the Where Used section as shown below.



Now I simply review all my actions and once satisfied I click the Perform Actions command.



Once the process is complete, I can exit the Revision Manager, and confirm my changes. I confirm that my OLD folder is now empty and that my New folder is populated with the newly named subassembly and its components.



I can open the assemblies in Solid Edge or Revision Manager to confirm that there are no broken links.


Although this was a simple example, you can see how this can be used on a larger scale. Revision Manager is a powerful and reliable tool that helps you manage your data in a non-managed environment. If your data has become too large to easily manage you should consider implementing Teamcenter.


Teamcenter is the world's most widely used PLM solution. For manufacturing companies who need to deliver increasingly complex products while maximizing productivity and streamlining global operations, Teamcenter helps increase revenue, get to market faster, reduce costs and improve product quality. Teamcenter simplifies PLM with targeted applications available to do what customers need when they need it. Platform capabilities get customers up and running quickly with a high definition user experience to inform decision-making anytime, anywhere. Applications are built on the PLM platform to help customers grow their deployment strategically over time.


For more information on Teamcenter, please visit our website at or contact us at [email protected]


How to: Reverse Engineer a Feature from a Round Surface

Manny Marquez - Tuesday, December 08, 2015


More videos here:

How to Search the Assembly Pathfinder for a Named Component

John Pearson - Wednesday, November 18, 2015

Solid Edge has a nice tool that can save you a lot of time if you need to isolate specific named parts in a large assembly. This tool is called Quick Query and can be found on the Select Tools tab of the PathFinder.



Let’s assume that you have to locate a component in a very large assembly. All you have is the component’s name to go by. Here are the steps to use the Quick Query to locate the named component.


  •    1.On the Select Tools tab, position your cursor over the Quick Query box, then right-click to display the shortcut menu.



   2.On the shortcut menu, set the Property option you want. In this example you need to select the Name property.



   3.On the shortcut menu, set the Condition option you want. You can set the condition to Contains, Is (Exactly), or Is Not.



   4.On the shortcut menu, click the Scope button to display the Scope dialog box, and then set the scope options you want.



Note: Solid Edge will remember the settings, so you only have to set them once if you continue to use the same property, condition and scope settings.


   5.On the Select Tools tab, type the value property you are searching for in the Quick Query box, and then click the Go button.



The parts that match the query properties you’ve defined are selected in the assembly window and PathFinder.




Note:Since the condition was set to Contains, it was not necessary to include the file extension. In fact, you do not even have to type the full name.


In this example, the Name property was used, but one could also search for components using any of the other properties listed in the quick query shortcut menu.


Quick queries are not stored on the Select Tools tab. If you wish to create a permanent query, click on the New Query button, on the Select Tools tab.




The Query dialog box will appear. Here you can define the query scope and criteria, as above, but you can also give the query a name. For example, below is a query, called Conveyor, which searches for the Category property which contains the word Conveyor.



Using this method saves the query in the assembly file for future reuse.



Queries can also be saved in the assembly template, so they can be reused in any of your assembly files, created from that template.

However you choose to use the queries they will provide quick and accurate search capabilities within your company’s assembly files.


How to Manage Dimensions in Draft Part 4

Manny Marquez - Thursday, November 05, 2015

Part 1:

Part 2:

Part 3:


More videos here:


How to save a flat pattern as a .dxf file in Solid Edge

John Pearson - Monday, October 26, 2015

In this blog, I want to focus on a single command; that being the “Save As Flat” command. I receive many calls from customers who ask how to create DXF files of their flattened parts. They need them to send to their manufacturing software or machine controller. Some have become creative and make a draft of the flat pattern and save that as a DXF file, but there’s an easier and better way. The best way is to use the “Save As Flat” command, using the following steps:

Once you have your sheet metal model created, create your flat pattern.I’m assuming that you already know how to create a flat pattern, so I won’t go into detail here.




Technically you can use the “Save As Flat” command to flatten the part, but I always recommend using the Flat Pattern command, to do this, for 2 reasons. First, you can verify that the flat pattern is feasible, and second, you probably need it anyway for your draft document.


Once you’ve created a flat pattern of the model, select the “Save As Flat” command from the pull down Application menu.



Notice that the “Save As Flat” dialog appears.



Before saving the file, click on the Options button, at the bottom of the dialog. This will launch the “Save As Flat DXF Options” dialog.



This dialog allows you to control what is output to the DXF file and how it is output. For example; if your controller does not like the bend centerlines output, you can block this by unchecking them in the Export to DXF column.



Now the centerlines will not be output to the DXF file when you save it.


Notice that there are 3 tabs in the dialog.



You can control Layers, Bend Data, and Fonts. If you are unsure of the settings you need, check with the machine operator or machine manuals. These settings are here only for controlling what is output into the DXF file. Therefore they have to match what your machine needs in the DXF file. If you want to read more about the options dialog, you can click on the Help button, in the bottom right corner of the dialog.


Once you set the options, click OK to return to the “Save As Flat” dialog. Select the folder that you want to save the file in, give the file a name, and make sure the “Save as type:” option is set to AutoCAD (*.dxf), then hit Save.



You now have a DXF file, of your flat pattern, to use in your manufacturing software or send to your machine controller.

Note: Once you set the options, in the “Save As Flat” dialog, they remain set. However it’s a good idea to document the settings in case your computer fails or you move to a newer version of Solid Edge.

Feel free to experiment with the options settings. Remember these settings only effect what’s output to the DXF file. They have no effect on the Solid Edge file.


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 [email protected]