More videos here: https://www.youtube.com/EdgeCanada
North America's Leading Siemens PLM Partner
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.
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.
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.
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.
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.
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;
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; http://www.designfusion.ca//technical-training.html. We can also arrange custom training to meet your company’s needs. For more information contact your Account Rep or contact us at firstname.lastname@example.org
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.
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.
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.
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.
•Draw Profile 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.
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:
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.
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.
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).
Check out our other videos : youtube.com/designfusion
(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.
Part 1: https://youtu.be/d3pXCcPMin4