move bodies

[rhoscadman]

Hi,

I am new to Inventor as our company leaders recently decided this is the way the dsign office should be heading. So, apart a basic inventor training week I have only used Inventor (Inventor 2013) in anger for the past 3 weeks. All is well and fine when it comes to building a part and then assembling it to other parts.

The problem starts when my engineer requirs a change in orientation for one of the components on the part. For clarity it is a pressure vessel with several flanges/spigots coming out of it.

I have manged to rotate a feature using the "move bodies" command around the central axis of the the main body of the vessel. But the sketch that I used to create this feature does not rotate with it. Why?

I have trawled the help line etc and still don't understand how to keep a feature and it's sketch together when I'm using Move Bodies.

Cheers

Rhoscadman

[nannerdw]

The Move Bodies command only moves the existing geometry.  It can't change the base sketches that were used to define that geometry.  There's no way to perform a "move" operation on a sketch, but you can redefine it to be on a different workplane.  Right-click the sketch in the model browser and select "Redefine"; then select a new plane for the sketch.  The workplane that you select must come before that sketch in the model tree.

Also, any subsequent part features that depend on that sketch may become broken and need to be re-created.

[gsmith9810]

Perhaps we're still having issues with terminology?

Assemblies are (for the most part) built up bu placing parts and constraining them with assembly constraints.

Parts are built up by placing features typically using a sketch on a face and then extruding or revolving the feature.

Bodies (to me) are typically IMPORTED from some external CAD system.

I would expect to build up a pressure vessel as an assembly of parts. 

[rhoscadman]

Perhaps we have different styles of designing vessels, and perhaps this doesn't neccessarily comply with Inventor's system.

The vessel we are designing is a flat bottomed steel tank with various spigots/flanges attached to it. Now the way I see it is that this vessel is one unit, flanges, spigots and penetration holes etcand would be built as a standalone unit, therefore I need to be able to manipulate the position of these attachements if need be. I see the point you're making but fear that our project admin would be overcrowded with "bits & bobs" that we have added to assemblies in the past and don't really understand what was used where.

Anyway, I'm losing track of what I'm looking for: simple manipulation of components/features/base sketches or whatever you want to call them.

I am attaching a copy of the part to maybe explain it better.

cheers

[Anonymous]

rhoscadman,

The easiest way would be to model each item (spigot, valve, flange, etc...) seperately and then create an assembly in which you bring in these pieces and constrain them to the tank accordingly.  This will allow more flexibility in moving them in various locations.  Of course the key here is being how well you constrain the parts with respect to the tank.  You can still move the items around within your ipt file, but more work is involved and you greatly increase the chance of having significant errors and problems in the future.  Think of it as a house of cards (there is an essay written regarding this analogy).  One error at the bottom of your design can cause several errors in other areas that can be extremely hard to diagnose and fix.

[gsmith9810]

One way to approach your problem would be to have a created library of iFeatures that create the individual spigots, flanges and penetrations you routinely use. You base feature would then benefit from having an appropriate number of reference planes positioned such that changing their location would be a simple matter of editing a dimension.

I suspect that my first inclination would be to approach the vessel as an assembly since it is going to be built as an assembly anyway.

Having created the final design you can always reduce the assembly to a part if that is what you feel the need to do.

Although I was able to see a preview of your part, I couldn't open as we're still running 2011.

- Gary

[Leanderjk]

+1 Gsmith,

I have to create a new line of warm water distributors in 10 different sizes pretty much every week, which is a breeze because I have a large library of parts I already designed for previous distributors.

You will have a larger amount of parts each time something new is designed but each physical part at your company is created separate aswell and all compiled into one product(the assembly) the same thing goes for designing products in Inventor.

[Leanderjk]

Adding to that, if you create a clean and ordered directory/library structure for all your designed parts your admin will see that it's a nice solution.

[johnsonshiue]

Hi! Move Bodies command operates the selected bodies at the state when the command is requested. The sketches used to build the bodies exist in prior states. As a result, they do not move along with the bodies later on. It sound like your design intent is to relocate features, not the bodies. If so, you can try Cut and Paste of features. You can simply select sketch-based features -> Ctrl+X and then do Ctrl+V by selecting a face to relocate. Depending on how you define the sketches, you might run into errors due to missing sketch planes. You can simply redefine the sketches by right-click on each sick sketch in the browser.

Please let me know if it works for you.

Thanks!

[rhoscadman]

Hi Johnson,

thanks for the info. I have tried the infamous copy/paste system, I trawled youtube and found an excellent video of how to use it, but have noticed that it on works on flat surfaces and not cylindrical ones like my vessel for some reason. I keep getting a "Unsatisfied Body Input" message come up. Oh well, never mind...........I'll just have to re model any features that need re positioning until I find a solution.

Thanks as well to all that have contributed to this thread.

Rhoscadman

[johnsonshiue]

Hi! You mentioned that you encountered some problem when doing Copy and Paste. Could you give me an example? I would like to understand the problem better.

Thanks!

[rhoscadman]

Hi, Thanks for getting back to me. I shall try to explain but forgive me if I'm not using the correct terminology.

I have been modelling a vessel about 1m in dia an have placed a manway access on, let's call it the 'south' side of the vessel. So I proceeded to cut a penetration hole on that face, then I offset the plane further out by 150mm and on this new plane I sketched and extruded a tube to meet the penetration hole. Then by the same process I fitted an ANSI 150 flange on top of that tube, complete with bolthole drillings etc.

My engineer came to me yesterday and suggested we reposition this whole feature (penetration hole/spigot tube/flange etc to the 'east' face.

So I realised I would have to create a new plane at a tangent to the east face. then in my browser I highlighted the ppenetration hole extrusion and right clicked < copy. Then I hovered on the workspace < right click < paste. And sure enough the sketch and projected geometry I used to create the original penetration hole appeared, as well as a dialoge box offering various options in Paste Features and Parameters. I select the ones I feel might br the correct one and then click finish. That's when the Incorrect Body Input message appears.

Does that help?

Cheers,

R.

[johnsonshiue]

Please do not worry about terminology. Your communication is very clear. But, I just want to make sure the behavior you see is correct but without an example part, it is very hard to tell. If you can share the part with me, please send it to johnson.shiue@autodesk.com. I am more than happy to take a look for you.

Thanks!

[rhoscadman]

OK, thanks. But I won't be able to do it any time today as I'm a bit behind in my work, so I'll try to forward you the file in the morning.

cheers

R.

[SBix26]

If you know ahead of time that you may need to change locations of manways, ports, etc., you could set up your model differently: use a sketch to specify the axis and radius of your port feature, then create the workplane for the feature from that sketch.  Then if you have to relocate, it means changing two parameters-- angle and height.  In the attached image, that would be the distance definition of the horizontal plane for height, and the sketch angle for radial location, since that defines the vertical workplane.

Sam B
Inventor 2012 Certified Professional

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