Autodesk Inventor

[#1]

Excuse me could someone tell me how to to make a part have different arrangements (eg a suppliers hydraulic cylinder extracted and collapsed) , and then show the  part in an assembly in the two different positions.  I am not sure if Iparts is the way to go, as I want both the arrangements to be displayed as the same part in the BOM....  the equivalent term is 'configurations' in solid works.

appreciate any assistance

[#2]

if it's the same part (ie the part doesn't change) in the assembly then can do it 2 ways:

1) position reps - can modify existing constraints to say show an arm in 2 positions.

2) presentation .ipn file and tweak existing constraints within the assembly, to move the parts about.  Arguably quite similar to position reps and yet another file to manage, but it's easier to use when moving lots of components, wanting to show trails (for exploded views) or wanting to move parts in a direction/rotation that isn't easy with the existing assembly constraints.

If you're trying to show an assembly in 2 positions with a changing component (e.g. spring in 2 states or say a wiring-loom in position a for assembly step 2 and position b when fully assembled) then it's a little more complicated.  If it's a sub-assembly then can consider using the "flexible" option and leave a constraint open (or with a max/min limit).  But if the modelling of the cad parts change then it's usually a little more complicated.  Personally create a second part with it in it's second state and insert that into the assembly next to the original and use position reps or a ipn presentation to toggle whether each version is visible for each state (and turn the altered part's visibility off in the BOM).

[#3]

Flexible sub assemblies for different positions of the same assembly.

Position Representations for drawing views.

Overlay view.

[#4]

Thanks for your response,

 your second paragraph is the scenario I am talking about.  I find the solution a little disheartening, In the assembly I will have 2 parts representing one part.  One being the correct part number, the other a piece of reference geometry, this will mean in one drawing view (with the reference geometry) the balloon items will not be parametrically driven.  The other concern is that if someone revises the 'actual' part in the future, the reference geometry part will be forgotten.

I guess there is no adequate work around in Inventor to replicate this solidworks functionality - so how do Inventor users get around this?  Does every moving mart have to be represented as an assembly? 

[#5]

lol...another solidworks can do this inventor cant post

no there is not a workaround

its a standard method

refer JDMAthers post or your VAR for proper training

[#6]

No, no, don't get me wrong, I think Inventor is as good as Solid works - if not worse. Stuart Cover Mechanical Designer BHP Billiton Mitsubishi Alliance Peak Downs Mine |Private Mail Bag, MORANBAH, QLD 4744 Phone: +61 7 4968 8218 I Mobile: +61 400 962 002 | Fax: +61 7 4968 8160 Email: stuart.cover@bhpbilliton.com [cid:image001.png@01CD552C.60BA0C60] Simply, the best people in coal. ________________________________ This message and any attached files may contain information that is confidential and/or subject of legal privilege intended only for use by the intended recipient. If you are not the intended recipient or the person responsible for delivering the message to the intended recipient, be advised that you have received this message in error and that any dissemination, copying or use of this message or attachment is strictly forbidden, as is the disclosure of the information therein. If you have received this message in error please notify the sender immediately and delete the message.

[#7]

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coves92 wrote:
No, no, don't get me wrong, I think Inventor is as good as Solid works - if not worse.

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that, my friend, I can accept

this link may help

http://wikihelp.autodesk.com/Inventor/enu/2013/Help/1310-Autodesk1310/1655-Assembli1655/1731-Represe...

[#8]

When do you have 2 parts in an assembly?  can you provide examples as there might be solutions (or alternatives to your present work-flow).

I only ask as your original post mentions moving cylinders which I would have thought should be a sub assy (with max/min limits within the constraints for the stroke).  This assembly gets placed in the main assembly and is set to "flexible" so it can move along it's free constraints.

The only times when you need 2 different versions of the same part is when the part physically changes like an o-ring in  its natural shape and then stretched when fitted.  Or, if you're explaining the steps of an assembly and needing to show how flexible components should be positioned at specific stages - e.g. a wire (built from a circle swept along a 3d-path) being fitted when the components are in 1 position in the build-process but those positions change when fully assembles and thus the wire's route changes accordingly.  With this in mind, going back to a moving piston, the parts do not change, so there shouldn't be a need for multiple versions of them within the assembly.

[#9]

Thanks for the reply, With supplier parts (for example a hydraulic cylinder), they may be made of many components, but our company only has one part number to order the complete assembly - so for simplicity I would model it as one part. That part would then have multiple versions (eg. retracted and extracted), that didn't create extra files and you could have two parts (in an assy) of the same name each displayed in different versions. Otherwise making an assembly of a supplier part adds extra complexity (adding mates, creating names for the reference geometry) when it is not needed. Eg if you were modelling an (off the shelf) engine, you wouldn't make an assembly creating all the bolts etc. However with inventor this cannot be done that way? If you create a part with multiple versions it creates another file for each version anyway? So at this point I am resolved to having to make an assembly (from reference parts) for any supplier part that moves, correct? Cheers Stuart Cover Mechanical Designer BHP Billiton Mitsubishi Alliance Peak Downs Mine |Private Mail Bag, MORANBAH, QLD 4744 Phone: +61 7 4968 8218 I Mobile: +61 400 962 002 | Fax: +61 7 4968 8160 Email: stuart.cover@bhpbilliton.com [cid:image001.png@01CD55C9.3EAB17C0] Simply, the best people in coal. ________________________________ This message and any attached files may contain information that is confidential and/or subject of legal privilege intended only for use by the intended recipient. If you are not the intended recipient or the person responsible for delivering the message to the intended recipient, be advised that you have received this message in error and that any dissemination, copying or use of this message or attachment is strictly forbidden, as is the disclosure of the information therein. If you have received this message in error please notify the sender immediately and delete the message.

[#10]

i would derive the supplier assembly into a part removing the piston and clevis.

I would also derive the assembly into a part of just the piston and clevis

break the links

then put the 2 parts together in an assy called your supplier part no.

you only have to add a couple constraints to make it work with flexibilty.

whole process should take you under 10 mins

then you only have 3 files to manage and dont have the overhead of all the suppliers IP

the link I gave you previously should point you in the right direction