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Extrusion in assembly

13 REPLIES 13
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Message 1 of 14
jbscott2121
5535 Views, 13 Replies

Extrusion in assembly

I was wondering why that when you are in an existing assembly, and you want to add something by extruding to one of the parts. The only option not greyed out is cut.
13 REPLIES 13
Message 2 of 14
JDMather
in reply to: jbscott2121

Just like the real world. You do not add material to an assenbly (except by weld or Move Face) you only cut material. If you want to add material to a part then edit the part.

Tip #95
http://home.pct.edu/~jmather/AU2006/MA13-3%20Mather.pdf

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Message 3 of 14
andrewiv
in reply to: jbscott2121

So why is it that we wouldn't be able to add surfaces to an assembly?

Andrew In’t Veld
CAD Administrator

Message 4 of 14
JDMather
in reply to: jbscott2121

Not sure what you mean. Faces or surfaces?

Simply Place Component and select the part with your surfaces.

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Message 5 of 14
andrewiv
in reply to: jbscott2121

I work in the conveyor business and we need to show the grade of the jobsite on our drawings. Most of the time I can just use the work planes to represent the grade, however if grade is different at the head of the conveyor then I have to create a part. It would be a lot easier if I could just extrude a surface in my assembly, rather than having an extra part file out there that will probably never be used again.

Andrew In’t Veld
CAD Administrator

Message 6 of 14
LFMarshall
in reply to: jbscott2121

UNlike the real world, i can't add stamping onto round parts at the assembly level which really irks me.
Larry Marshall
Inventor 2021.2 , AutoCAD 2021, 3DS Max 2021
Message 7 of 14
Anonymous
in reply to: jbscott2121

Just create a sketch, or even better, create a skeleton, a IPT that only has
a sketch that is your grade. You will be able to contrain items to the
skeletal sketch. If your grade changes, so will your conveyor.

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wrote in message news:5865626@discussion.autodesk.com...
I work in the conveyor business and we need to show the grade of the jobsite
on our drawings. Most of the time I can just use the work planes to
represent the grade, however if grade is different at the head of the
conveyor then I have to create a part. It would be a lot easier if I could
just extrude a surface in my assembly, rather than having an extra part file
out there that will probably never be used again.
Message 8 of 14
pcunningham1
in reply to: jbscott2121

You'd think you could use assembly sketch geometry to define assembly work planes, and thus not need the phantom/skeleton part, but you'd be wrong!

-Paul Cunningham
Paul Cunningham
IV2008
Message 9 of 14
Anonymous
in reply to: jbscott2121

The nice thing is that you can change the BOM to reference for the skeletal
IPT and not have it show up.
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Dell 670 dual Xeon - 3.2
3gb memory, SCSI320-15k
XP-Pro, sp2
Quadro FX3400: Driver: 169.61 Direct3D
IV2008-pro sp2,
SpacePilot Rel V: 3.5.4 Dvr V: 6.4.4 Firmware 3.12

wrote in message news:5866196@discussion.autodesk.com...
You'd think you could use assembly sketch geometry to define assembly work
planes, and thus not need the phantom/skeleton part, but you'd be wrong!

-Paul Cunningham
Message 10 of 14
Boorda
in reply to: Anonymous

The skeleton approach may work for some companies, but not for all.

For example, we do not directly insert skeleton files into our assemblies, we only include skeleton file parameters by linking through the parameter table. One reason for this is because we use a breakaway skeleton method in which the skeleton file is removed once the project is completed. This evolved from problems of skeleton files accidentally be changed and inadvertently updating other projects due to copy design issues from Vault. Linking the skeletons to many parts and assemblies via the parameter table allows the parameter name and dimension to remain intact and convert to manual entry parameters when the skeleton file is detached. When the skeleton files were included directly in the assembly and we removed the skeleton file from the project unresolved reference errors occurred on multitudes of assemblies within the project.

Bottom line is that a lot of people are asking about this and it would be nice to be able to extrude a surface in an assembly as a work feature. In a large company where we deal with thousands of parts efficiency is a huge issue. It's not very efficient to have to create an extra file for those who don't need to. It also leaves the door open for one more element to fail if that skeleton gets deleted or corrupt as opposed simply including the surface data in the assembly file with the other work features such as planes and axis.


Automation is key!
Message 11 of 14
JDMather
in reply to: Boorda


@Boorda wrote:

Bottom line is that a lot of people are asking about this....


http://forums.autodesk.com/t5/Inventor-IdeaStation/idb-p/v1232

 


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Message 12 of 14
jrspath1
in reply to: jbscott2121

I agree with this comment.  I had a large assembly and only wanted a small part of this to make an exploded presentation file to put in an instruction manual.  The only way I knew to do that was to enclose a shape around the small part I wanted and delete the remainder of the assembly outside of this shape.  If Inventor wants to remain relevant then things like this should not happen.

Message 13 of 14


@jrspath1 wrote:

I agree with this comment.  I had a large assembly and only wanted a small part of this to make an exploded presentation file


Hi jrspath1,

 

If I'm understanding correctly, it sounds like creating a View Representation in your assembly file first, and turning off all but the small part of the assembly you wanted to show in the exploded view, and then creating the Presentation file using that View Representation, would have been the best method.

 

In any case this discussion topic is quite old and originally discussed the ability to add material with an assembly level extrusion. Your post sounds like a different topic, so feel free to start a new discussion, and I'm sure someone will be able to assist.

 

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com

Message 14 of 14
anuarenrique
in reply to: jbscott2121

The top-down design methodology, being best for working on an assembly, indicates that the parts are created directly from this environment by having one of the parts as reference.

 

So just create this new ipt and joint it where you want.

Si mi respuesta te fue util agradezco tus kudos y en caso de resolver tu problema recuerda aceptar como solucion. Gracias.

Apoya nuevas idas. Aprende todos los dias. Ayuda a todos!

Anuar Mata
Autodesk Student Ambassador
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