level of detail - suppress extrusions?

[Anonymous]

Hey guys,

Seeing as everyone is so much help I thought id ask another one.

Im doing up a handrail for work. I need green left on the item for when it is pressed so have drawn it as such. Now I have to cut the green off which ive done using a simple rectangle extrusion. 

Is there any way I can get a level of detail or positional view setup so when I insert it into my main assembly it can be the correct size peice but when I create my idw I can have the actual size they will need to press?

I read something about turning it into a weldment which I have done (easy enough to redraw if I need to get it back to a normal assembly). Cant seem to get this to work. 

Thanks

Brad

[blair]

If it's a IAM, you could use a Assembly Feature. It only resides in the Assembly IAM and not in the IPT file/level. Any IPT drawings won't have the Assembly Feature in them. It can also be suppressed in the IAM level as well with View Reps.

Weldments are a one-way conversion. Once you convert to a Weldment, you can't convert back short of restoring from an "old version".

[Anonymous]

Its a simple U shape peice of pipe used as a foot step so if I needed to convert back I would just delete it and start again. 

I think the problem I am having is that it is a frame generated component. 

The peice is 25NB med black pipe (33.7x2.5 wall in the AS section of frame generator) 450 wide with 250 legs, 107mm CL radius bends to 90degrees.

That will allow my machine to bend the shape. Once it is bent they have to cut the legs back to an overall height of around 100mm. 

Ive used position and representation heaps lately with assembled parts and constraining into different areas but there is a few items I have to allow for green with when pressing/bending which I feel are going to come up soon so hoping I can set this up to save designing the part twice. 

If I used position representation it wont allow me to suppress a extrusion. If I use a level of detail it suppress/unsuppresses in both LOD's. 

[blair]

Easy, if it's an IPT file, delete the extrusion and place it in an IAM file and save it with the same file name, it will have a different extension. Use the IPT in the drawing for the "Green" length. When it's in the IAM file, create an Assemble feature and cut it to the end length. Then use the IAM file for the drawing with the finished length.

You could also do this as a Derived part.

If it's a Frame-Gen item it will be in a IAM file and the Assemble cut Feature will work there as well. Use the IPT for the "Green" length.

You can't suppress Features within a IPT.

I think it might be easier to go with the IPT for your drawings to the shop to bend the "U" and then place it into a IAM file and use the Assembly Features to "Trim" the legs. This way the Assembly Features don't migrate back to the IPT and only reside in the IAM. Then use the IAM with the single IPT in it for your work.

[SBix26]

Another possible solution is to use multiple solids, though I'm not sure how this will work with Frame Generator:

In your finished part, add the additional 'green' lengths as new solids (you could even give them a green appearance to make their purpose clearer).  Create a View Representation named Trimmed or Finished, or something like that, and turn off the visibility of the added solid bodies.  In your Frame Generator assembly change the occurrences of this part to use the Trimmed view rep.

In the drawing, you would use the Master view rep, but could add hatching to the 'green' areas to indicate the trim operation.

Sam B

Inventor Professional 2017.3
Vault Basic 2017.0.1
Windows 7 Enterprise 64-bit, SP1
Inventor Certified Professional

[SBix26]

Just tried a quick test with Frame Generator - seems to work fine.

Sam B

Inventor Professional 2017.3
Vault Basic 2017.0.1
Windows 7 Enterprise 64-bit, SP1
Inventor Certified Professional

[mcgyvr]

Sounds to me like this should be an "ipart"...

I do that all the time when I have a part that (for example) I need to show on my drawing in a "flat" state yet when it is actually assembled they fold it in half and use it that way..

I have 2 members in the ipart.. 1 with the fold there and 1 that suppresses the fold..

[Curtis_Waguespack]

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@mcgyvr wrote:

Sounds to me like this should be an "ipart"...

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Nope! It should be a part level LOD .

http://forums.autodesk.com/t5/inventor-ideas/level-of-detail-for-parts/idi-p/3822718

My understanding is that part level LODs are being considered for future versions of Inventor, but until then iParts , Derived parts, weldments, etc would be a good way to go.

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

[mcgyvr]

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@Curtis_Waguespack wrote:

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@mcgyvr wrote:

Sounds to me like this should be an "ipart"...

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Nope! It should be a part level LOD .

http://forums.autodesk.com/t5/inventor-ideas/level-of-detail-for-parts/idi-p/3822718

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Same dang thing.. 

[Curtis_Waguespack]

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@mcgyvr wrote:

Same dang thing.. 

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Technically your left shoe and your right shoe are the same dang thing too.  

LOD for parts will be like having one quantum shoe that fits perfectly on either foot, and can exist on each foot at the same time.

[mcgyvr]

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@Curtis_Waguespack wrote:

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@mcgyvr wrote:

Same dang thing.. 

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Technically your left shoe and your right shoe are the same dang thing too.  

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So your the guy I always see around with the toes pointed outward walking like you have a load in your pants.. 

technically.. smechnically.. 

[Curtis_Waguespack]

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mcgyvr wrote:

So your the guy  ...  

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 LOL.... no, I think that's just a mirror that you're walking by.

[mcgyvr]

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@Curtis_Waguespack wrote:

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mcgyvr wrote:

So your the guy  ...  

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 LOL.... no, I think that's just a mirror that you're walking by.

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A "mirror".. I'll give you that.. A left is technically a mirror of a right shoe..

I did have "special" shoes when I was a newborn so watch it buddy

[Curtis_Waguespack]

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@mcgyvr wrote:

... A left is technically a mirror of a right shoe... 

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I forget who it was, but someone once said, "technically.. smechnically." 

@ brad91, it appears your thread has been hijacked by nonsense!

Feel free to get us back on track if you need further info about your suppress extrusions question... or about mcgyvr's childhood.

[Anonymous]

Thanks guys,

I got side tracked and dragged off this project for a bit. Ill have another look at it shortly. Doing my head in working on 5-10 different projects at once haha