Inventor: Multi-Body Part Modeling (Part 2 of 2)

Posted on August 5, 2014 by Dave Breiner, Synergis Solutions Engineer:

In Multi-Body Part Modeling (Part 1) we left off with our completed Master Part. You will now move onto creating the assembly and parts, manipulating the Master Part and any clean-up and setting of iProperties.

This portion of the tutorial will cover:

  • Creation of Assembly and Parts from the Master Part
  • Clean-up of the Parts by setting iProperties
  • Manipulating the Assembly by adjusting the Master Part

Creating Assembly & Parts from the Master Part

Creating your Assembly

Fig. 18

Fig. 18

From the Master Part in (fig. 18), you will create the assembly as noted in (fig. 19). Solids will be selected and will become new parts in individual IPT files which are automatically inserted into a new assembly. The new IPTs will retain their link to the Master Part through derived links.

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You will begin the process from the Master Part by selecting the Make Components command located on the Manage Tab and the Layout Panel (fig. 20). The Make Components: Selection window opens (fig. 21).

 

Begin by selecting the Solid Bodies, from the model browser window that will become parts in the new assembly. At this time, you can change the assembly name and/or the assembly location in this Selection window (fig. 22). Click Next after all of your Solid Bodies have been selected.

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Clicking Next will allow editing of the Component Names, Template for the component, BOM structure, individual source paths, Scale Factor, Mirroring and Parameter passing to the children (fig. 23). For this example, you will accept the names as they exist.

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Selecting OK will create an assembly with all the bodies as New components grounded together at the Origin of the assembly (fig. 24).  Save the assembly to actually create the new .ipts and .iam in the workspace.

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Okay, you’re done right? I don’t think so!

Let’s take a look at the assembly and see what we have.

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Taking a look at the browser (fig. 25), you will see that all of the solids have come into the assembly as separate parts.

All of the parts are grounded to the origin. This eliminates the need for constraints.

You can now open each part and fill out our iProperties.

 

* mbb9Before you get into the iProperties, there is a little trick I would like to share with you that I find to be a big help. I find it a good practice to place the Master part file into the assembly. This makes it much easier to access when you want to adjust the design and it also tells others working with the assembly that it is a multi-body design. This process also helps to keep the Master Part with the derived assembly.

In Fig. 26 I have added the Master part to the assembly and selected “Place Grounded at Origin”. This will lock the part to the origin and add it at the bottom of the browser.

mbb10After placing your master part into the assembly and grounding it to the origin, you need to RMB on the part and select “Reference” from the BOM Structure flyout. This will ensure that the Master Part does not show up in the Parts List.

RMB a second time and select Suppress (fig. 27). This will make the Master Part available to open from the assembly for quick editing.

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As an added help, you can add a Folder and place the Master Part in it as I have done at right in fig. 27A. You can then slide the folder to the top of the browser list for a higher profile and easier to see.

Clean-up of the Parts by setting iProperties

The most common first step is to assign Materials. You can always go the usual route and open each part to set up the iProperties, as shown in (fig. 28).

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A MUCH faster way is to enter all of your iProperties information at one time from the Bill of Materials command. From the Manage tab and the Manage panel, select the Bill of Materials command.

mbb13From the Bill of Materials window you can enter all of the iProperties information at one time.  Select the Column Chooser from the menu bar at the top of the page.  From the Column Chooser window select which iProperty you want and drag it to the desired position as I have (fig. 29.)  Now you can go part to part and set your iProperties from one location.

It is also a simple matter to go to each part then select any appearance that you wish (fig. 30).

mbb14Manipulating the Assembly by Adjusting the Master Part

Let’s go into the Master Part and make a few changes and track them through to the assembly.

1.    I will add a few chamfers to the part.  The nice feature here is that instead of opening every part to add chamfers,  I can apply all of the chamfers at one time and have them applied to the assembly.  As you can see in (fig. 31),  I have applied several chamfers to several solids.  This would take three separate operations in a typical assembly, but only one operation here.
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Save the part and go to the assembly.  Click the update button and your assembly will update with all the applied chamfers. (fig. 32)

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2.      For the next change I will start in the master part and making several changes, base length, base width and head position (fig. 33) from the iLogic form, then click Done and Save.

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Going to the assembly and selecting update applies the changes. (fig. 34)

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As a last note, I would like to point out that you can always add additional Solids to your Master Part. You will need to go to the Manage tab and the Layout panel and select the Make Part or the Make Components command to add these solids as parts to the current assembly.

This brings us to the end of this tutorial.  By now you should have a good idea if Multi-Body Part Modeling is a value to you and your process.  It certainly is another tool for your design tool box that you may apply to help reduce time and errors.

Until next time…

DLB

dave_breiner_MG_0352Dave Breiner joined Synergis in 2013 as a Solutions Engineer on our Manufacturing team with an amazing amount of experience. Coming directly from being a CAD Manager with SPX/Ecolaire, Dave is well versed in implementing and using Autodesk software having transitioned the department from 2D to 3D modeling by developing a 3D modeling program, implementing modeling standards, and creating automated models using iLogic programming. Dave began his career with SPX as a preliminary designer of steam condensers before being promoted to Manager of Drafting. Prior to this, Dave was with Bethlehem Steel for over 20 years, performing many tasks including millwright, rigger and fitter. During this time he also completed his degree in Engineering Design.

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4 comments

  • Hey there! I’ve been reading your web site for a long time now and finally
    got the courage to go ahead and give you a shout out from Kingwood Texas!
    Just wanted to say keep up the fantastic work!

    Like

  • Thanks for your time in putting this article together. I tried using this technique several times (IV 2012) and came to view it much like I do iMates, mainly because of the issue of having to manually rename all the generated parts to something more meaningful. Now that I know renaming the solids is what will transfers to the new assembly file, it’s a lot more useful.

    Like

  • Hey Dave, It’s really helpful, What if I want to add Plane from master model to Assembly? I’m new in Inventor, so I didn’t find the way to import Planes or sketches from master model.

    Thank you

    Like

  • Hi Dave, thank you very nice for your articles, best on this blog. Very interesting reading. I’m looking for next.

    Like

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