Hole not "Through All"

Anonymous · ‎09-22-2015

Hi,

Ill try to explain this issue quick.

I have an adaptable assembly. I have created a workplane where I want it with a sketch and a fully constrained construction point. A hole is made from this point location and I have set it to go "Through All" components of this assembly. When I first build the hole, it works great.

Since the assembly is adaptable, when it grows more pieces are added in which the hole must also go through however when the assembly grows, the hole does not adapt properly. I have found the "add participant" option but to me this is just another annoying manual workaround for these types of problems.

I am in the process of trying to make my assembly 100% adaptable through use of iLogic and this is just another hiccup. If anybody knows if there is a way to get the result im looking for I would really appreciate the help!

Im using Inventor 2016 btw..

Thanks

Sandro

JDMather · ‎09-22-2015

How/when is this hole made in the real world?

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Anonymous · ‎09-22-2015

The holes are plasma cut through each piece before they are all welded in place. The reason for the hole is because a piece of pipe will be running through each piece. More pieces = more holes.

blair · ‎09-22-2015

All that I can think is to create an iLogic with the trigger when another part is added to the assemble, this "Assembly Hole Feature" refreshes it'self. I don't even know if that is doable with iLogic.

You might search the forum looking for iLogic guru's and send them a private message if this is even doable. I don't spend very much time in iLogic.

The problem is that the feature must be "refreshed" each time a new part is added.

You will then need to push this Assembly Hole Feature down to each IPT for it to then show up on each IPT when they are opened individually as well as when drawings of the IPT (at the part level) are generated.

Inventor 2020, In-Cad, Simulation Mechanical

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Anonymous · ‎09-22-2015

Thanks for the reply. I have tried what you mentioned using what I know about iLogic. I created the rule..

If (something obvious) Then
Hole = false
End If
If (something obvious) Then
Hole = True
End if

I figured this would regenerate the hole feature but it did not work. I might be on to something if i can get the rule to run at the right time but as for now im still stuck. Could you refer me to an "iLogic guru" if you know one please?

Thanks
Sandro

blair · ‎09-22-2015

Search this forum for iLogic in the Seach box at the top of the web pages, also Curtis Waguespack is pretty good with iLogic as well.

Inventor 2020, In-Cad, Simulation Mechanical

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PaulMunford · ‎09-22-2015

Could you derive the hole instead?

Paul Munford
Technical Onboarding Architect
Linkedin

Anonymous · ‎09-22-2015

Paul,

I am not sure what you mean by that

Anonymous · ‎09-23-2015

Blair,

I tried to take your advise and contact this Curtis character but he has his private messages turned off. I am new to this autodesk site so I am kind of lost as to my next steps..

Do you know of any other users of iLogic that might be willing to help me?
I really appreciate it

Thanks
Sandro

blair · ‎09-23-2015

As I posted, use the "Search" function in the upper RH corner of these forum web-pages and search for "iLogic". Look for the posted answers and who supplied them. Try contacting those that have supplied great iLogic examples and solutions.

Inventor 2020, In-Cad, Simulation Mechanical

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cwhetten · ‎09-30-2015

Hi Sandro, are you still trying to get this to work or did you find a solution?

Cameron Whetten
Inventor 2016

Anonymous · ‎09-30-2015

Again, thanks for the reply Cam!

I have put this issue to the side as I have with many others because it is not directly affecting my work...yet.

I am still looking for a solution though to answer your question.

Thanks

Sandro

Curtis_W · ‎09-30-2015

Hi bnwtech,

If I understand correctly, these links might help:

http://forums.autodesk.com/t5/inventor-general-discussion/is-there-any-better-way-to-add-and-remove-...

http://forums.autodesk.com/t5/inventor-general-discussion/ilogic-commands-for-adding-a-participant-t...

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

SteveMDennis · ‎09-30-2015

Sandro,

The reason we do not automatically add everything to an assembly feature is performance. Through all at the time of creation will add all affected components to the hole feature. We make this as fast as we can by using bounding boxes, etc. but once we gather the list of everythign affected future computes use those participants only.

To do what you expect everytime the assembly computed, had anything added, moved, etc. We would have to exhaustively recalculate that particpant list again. This would adversely affect EACH assembly solve if we tried to keep your list dynamic like this.

This is the rationale behind our original design.

Peeking at the threads mentioned above you can get around this if you desire, but if you add a participant that will affect compute time even if the participant is miles away from the hole, that is the downside of adding every new occurrence to the hole feature.

Just wanted to share the history and a bit of the reasoning here. You are free to add an IdeaStation topic for this but in a large assembly the performance might be very bad...

Steve Dennis
Sr. Principal Engineer
Inventor
Autodesk, Inc.

Anonymous · ‎09-30-2015

All,

Thank you for the tips and advise, I am not sure i will have the time to check out the links today however I am really looking forward to it so i might be able to get past this.

Thank you Steven for the rationale. I think i understand what you are saying here although I still think I will want to achieve my desired result if the provided links show me how.
The hole will only ever be going through 1 more component (pattern) so there may be 1 - unlimited amount but it is still within one component. I am not sure if that makes a difference..

I will let you guys know how it goes.

Thanks for the help!

Sandro

Anonymous · ‎10-01-2015

Curtis,

I looked at the links and it helped a lot. I read through the whole conversation and it actually gave me a way better idea rather than using code. I actually feel pretty silly now...

I am not even going to bother using that block of code you mentioned as what I am trying to do can be accomplished much easier. I will simply add the hole to the component that is used in my pattern and it will duplicate itself that way. I can simply create a rule to suppress that particular hole when its not needed and therefore suppress all other holes in the pattern.

Thanks for the help! I really appreciate it.

I also read in that conversation that "these types of questions are better posted to Inventor Customization." Is this true? Could this be why I seem to be having trouble finding the best solutions to my iLogic problems?

Thanks

Sandro

Curtis_W · ‎10-01-2015

Hi bnwtech,

I prefer the Inventor Customization forum for programming and automation questions, but people seem to post iLogic related questions on this forum and the customization one, so I tend to search both of them.

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

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Hole not &quot;Through All&quot;