Multi-Body Modeling in Solidedge
How To Do Multi-Body Modeling in Solidedge
Get ready to take a look at what our experts like to call the “hidden gems” as I walkthrough multi-body modeling in Solidedge. These are extremely powerful tools that you can utilize for better efficiency and effectiveness among your team.
What is Multi-Body Modeling?
Multi-body modeling is the ability to design multiple pieces or multiple parts within the context of the same part file. With this type of environment, you can design many separate models in the same space and according to the same set of rules. This method provides the ability to model many components of an assembly as a single part or sheet metal file. We can have a multi-body part that has a single part, or if we choose, we can have it broken out into a separate assembly where it is being controlled from the master part. Multi-Body Modeling in Solidedge is a useful feature that has the ability to capture that information and help you utilize that data within a single part model.
Things to Know
- Can be a part or sheet metal model type
- Can contain both ordered and synchronous features
- A part design body can contain a single solid or disjoint solids
- Sheet metal design bodies do not support disjoint solids
- New design bodies share existing material properties of the initial design body
- You can switch a design body to a construction body
- Construction bodies have their display turned off by default in assembly or draft file
- Construction bodies display with the construction color (purple)
- Construction bodies do not publish
How to Add Multi-Body Modeling Parts
This is a regular plate with no additions. I already created one of the plates needed on the left hand side.
- From the actual part environment, click Add Body and choose the type of body you want for this multi command: either Part Body or Sheet Metal Body. Click OK.
This will pull out a template from the Edit default creation templates.
- Get the outline of the of the sheet metal part that you want to create.
- By using Project Sketch, trim up the edges, and use the Contour Flange to trim, extend, and set the thickness. Give it the depth or the width of the actual sheet metal component part.
- Now, you can finish off the design. Let’s say you want to go ahead and cap both of the ends to get a protective case around the tooling piece- you can still use the synchronous sheet metal components.
In this case, this is considered a sheet metal file when I’m in activated with it activated within this part. All the commands will still behave the same way as they would as if it was an independent part and I was bringing it into an assembly.
- Pull some tabs down and grab the Flanges to display a cap. Duplicate that over to the other side so you can have right and left hands. Once it is prepped with a mirror, select the part that you want to copy over and then go into your mirror command.
You may notice an error that will pop up when you try to do this. This error is going to tell you that you can’t do it. That is because it is a sheet metal component piece, and you cannot have disjointed pieces. Instead, detach the face so it will copy over it as a construction body. This is how you can get around the disjointed body issue.
- Once it is a construction body collection of surfaces, right click and Toggle it into a Design Body. It will then change colors as it moves into your design body container within the Pathfinder.
- Rename it.
- Now, you have your new two sheet metal pieces. The next step is to rinse and repeat what is on the plate, and the first thing you want to do is activate it by clicking Activate Body.
You’ll notice the color shift from a dull color to a brighter color. That will be your indicator that it is actually in place activation within that part.
- You can follow these same steps with the other part by toggling it to make it a design body, then rename the component piece. This will be your right plate.
- If you want to take it into a drafting file, first you’ll want to activate the main body. You can also designate it as your assembly body by just right clicking and clicking Activate Assembly Body.
- Click Save. This will represent your Multi-Body Modeling Solidedge Assembly.
Adding Your Multi-Body Modeling Parts Into a Draft
- Click Open, then New Drawing of Active Model, and click OK. Now, you will want to drag your model into a Draft with ISO View.
The way that it is going to get placed will still resemble a part file, which will end up being one single entry, as Solidedge is still a single part file. It has multiple bodies in it, but it’s not going to recognize any of the new parts that were added in.
- Go to Home, then Parts List, and then adjust settings as needed. This will give you a part number or the part name for the main component piece, with no other details.
Creating a Multi-Body Assembly
- Click Multibody Publish. This will separate components into each individual part files, and then it will allow you to go inside the draft too.
- Click on Set Path to set a path directory.
You can select all of them and this will create your assembly. After you save the files as what we like to call a “Dummy Assembly, it will create a link between this part and each one of these subcomponents that it’s saving. You will see a link signifying that the two parts are linked. Now, this will become the controlling master file. If you need to make any changes, make it to this particular file so it will publish any changes necessary.
- You can now open the Dummy Assembly you just saved to see all of your component pieces listed, along with your one to two extra pieces that were made.
Placing the Multi-Body Modeling Assembly Into a Draft
- Go to ISO View.
- Place the Assembly design into the Draft, and click Parts List. You may have to change the configurations.
- Go back to the original part (remember- this is the one driving the rest of the the rest of the model.) activate a part by right clicking, then Activate Body.
- You can drag this face out or mirror the plane, and then you will see that both sides will automatically change.
- To automatically update and publish this out as a Draft file, click back to your original part and click the command underneath Add Body called Multi Body Publish.
- You will notice that the left bracket will have clocks on them as well as the assembly. Click on each clock to update it and then click Save Files.
- If needed, go back to the Draft file and open the Assembly again, then click Update Views to ensure the draft is updated as well.
- If a pop up occurs, click Clear All and then Close.
The draft file will have updated the changes.
Straight from our expert, this is one of the most powerful hidden gems that will help you navigate through Multi-Body Modeling in Solidedge, and will certainly become a great resource for you and your team. For more tips on using Multi-Body Modeling in Solidedge, be sure to click here and watch one of our other helpful demonstrations.