Community
Inventor Forum
Welcome to Autodesk’s Inventor Forums. Share your knowledge, ask questions, and explore popular Inventor topics.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Top-Down Assembly Strategy / Frame Generator Features

13 REPLIES 13
Reply
Message 1 of 14
emil.cashin
723 Views, 13 Replies

Top-Down Assembly Strategy / Frame Generator Features

Hello,

 

I'm a relatively new Inventor user (experienced SW user still figuring out the different approaches needed in Inventor) and am having some trouble with top-down design. I have an assembly that is essentially a parametric Frame Generator assembly with some assembly features (cuts, holes) and a few other parts. My problem is getting assembly features to update parametrically, since Inventor doesn't allow parametric projection of geometry. I need this assembly to be easy to work with parametrically because I make a copy for individual clients and tailor the geometry to their needs, and obviously want to spend time on getting the numbers right instead of fixing broken sketch relations.

 

Here's my strategy and understanding of what's going on:

- I have a frame layout sketch as a part file, which I place in my assembly and use to build the frame.

- I have center points on the frame layout sketch (at part level) for holes, profiles for cuts, etc.

- In order to make these holes and cutouts, my approach was to (at the assembly level) make new sketches, project geometry from the frame layout sketch, and make the features from that geometry. Obviously, this approach fails because the sketch projection is not parametric.

 

I can probably kludge something together by linking my driving Excel file to all the frame member parts individually, but it seems like I must be missing a reasonable way to make my subtractive features from the frame layout sketch geometry and have them update parametrically. I'm open to other approaches, but due to the structural sections involved I'm fairly wedded to Frame Generator at least.

 

Thank you for any advice!

13 REPLIES 13
Message 2 of 14
cbenner
in reply to: emil.cashin

Welcome Emil,

 

Can you post any shots of what you are trying to do, just for visuals?  Also, to clarify... you are projecting from the original frame sketch to create assembly features.... what is it that is NOT hppening when you do this?  Are you trying to change the base sketch and have your holes follow?  Maybe you want to project geometry from the frame members themselves?  Also, have you tried to do a "Rebuild All" at the top level, (and at all sub assy levels) to see of things update?

Message 3 of 14
jeanchile
in reply to: emil.cashin


@emil.cashin wrote:

.... since Inventor doesn't allow parametric projection of geometry.


I'm with cbenner on this. This phrase of yours is throwing me. I think we do something very similar to what you are asking about here but more information is needed to help out with your specific situation. Any chance you can create a simple data-set that has all of the ideas you talking about and throw it up here? Are you familiar with "adaptivity" in IV (may not be the best solution which is why I ask for more info)? Are your holes and features at the assembly level or part level?

Inventor Professional
Message 4 of 14
emil.cashin
in reply to: emil.cashin

Ah, I could have been much more clear. Let me try again:

 

In the most basic case, I want to make a frame member and put a hole in it, with the member length and hole position parametrically driven.

 

My current strategy, which doesn't work, is:

- Make a frame layout part with a line sketch for the frame member, parametrically defined.

- Open this part in an assembly, fire up Frame Generator, and make my line sketch into a frame member (or set thereof).

- In the assembly, make a new sketch and project geometry from my frame layout part to locate the hole(s). Say I just project the frame member line and dimension a point on it. I can do this either within the frame or at the top level of the assembly - if I do it within the frame, the resulting features will show up on the frame member parts when opened separately - but neither approach works for parameterization as I'll describe.

- Make a hole or cut feature from that new sketch.

- Change the frame layout parameters to move the hole (hole doesn't move).

 

Because I projected sketch geometry from a part (my frame layout sketch part) to the assembly level, Inventor adds a fixed constraint to the projected geometry rather than a projected constraint, and so parametric changes do not affect the projected features (because they're not "projected", they're fixed after being projected the first time). This was a surprising behavior to me (coming from Solidworks), and threw a wrench in my strategy.

 

 

 

My temporary workaround is to make the same frame layout sketch (driven parametrically by the same Excelsheet) at the assembly level and make my assembly-level features using that. Since I then can do all my geometry-projection (for various feature sketches) at the assembly level, all the projected entities are still parametrically associated. The problem then is just that I have two identical sketches to drive my features, which means that I have to change both whenever I want to add something. It's not awful by any means, it just feels like a kludgey solution to a really simple task and that there must be a better way. Can I derive my assembly-level layout sketch from the part-level sketch?

 

Having figured out at least how to move forward, I'm still looking for a better approach. When I do top-down design, I want to have a single layout that drives everything. Using Frame Generator forces that layout into a part that is brought into an assembly, and thus I can't project properly from my layout. Perhaps I'm being overly obsessive about having an elegant approach, but as a relatively new Inventor user I'm very curious to learn the best practices for how to go about these things.

 

Thanks for bearing with me!

Message 5 of 14
emil.cashin
in reply to: emil.cashin

Here's a project that shows the behavior. I have a frame layout part driven by an Excel file, and an assembly in which I've projected a hole. I then changed the parameters and of course the hole position didn't update because the relation in the assembly is set to fixed.

 

I would love to hear a good reason for why Inventor works this way, but what I'm really after is the "correct" approach to these situations!

 

Coming from Solidworks, I'm perhaps used to being able to get away with things in that you can kind of stick everything together and it'll cope, though that's not to say that doing so is good practice.

Message 6 of 14
cbenner
in reply to: emil.cashin

Hey,

 

I was able to get this to work by adding the hole at the Frame assy level: (Frame0001).  I had to link the Excel file at that level as well so the hole parameter was at that level.  I then changed the parameters (both of them) several times, and did a Global Update form the top level and everything updated as expected.  At the Frame0001 level I added the 2D sketch, projected the frame_layout sketch and added a point just as you did.  Then still at the Frame0001 level I added the hole feature and the parameters linked to your Excel file.  It doesn't seem to hurt anything that the same Excel is linked at different levels of the assembly.

 

I don't do this very often since most of our designs are fairly rigid...so this may not be the most elegant solution, but it did work!  LOL

 

btw, I did this is 2015.

 

toy.JPG

Message 7 of 14
emil.cashin
in reply to: cbenner

Ah, interesting. I think that's roughly equivalent to what I'm doing now, in which I link parameters to my assembly and make a new, fully dimensioned and parameterized sketch.

 

When you project the layout line in '15, does the projected line change length when you update parameters? My understanding is that it doesn't despite what I think it ought to do. I'm in '14 and I doubt they changed that behavior.

 

Thanks for taking a shot at it! It's certainly a workable approach.

Message 8 of 14
cbenner
in reply to: emil.cashin

The length of the projected line did not change, but the location of the point defining the hole does.  Did you place this point in your new sketch, or was it in the original sketch and then projected to the new sketch?

Message 9 of 14
serpennica
in reply to: emil.cashin

one tip that may help, Inventor does not like to use projected geometry from a part surface. You will always loose that surface reference when you change frame member.  If you can setup working planes to establish your member length and hole position then the frame generator part does not get affected. You could use the excel spread sheet to change the dimension of working planes and the frame member part and hole will follow.

Message 10 of 14
johnsonshiue
in reply to: serpennica

Hi! I could be wrong but I am not sure losing projected surface reference is the right behavior. Could you share an example that illustrates the behavior? I would like to understand it better. There might be a bug here.

Many thanks!



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Message 11 of 14
serpennica
in reply to: johnsonshiue

Will post again after holiday.
When using projected geometry from an extrusion. If the extrusion is rebuilt with new parameters the projected sketch geomentry will be have error.
Message 12 of 14
serpennica
in reply to: emil.cashin

i made this a little simple to work with, I have working planes to measure with that makes it simpler to see.

I am trying to keep the work planes at 90deg to each other and if possible 90deg to origin planes. One end at 6ft x 3ft is different size then opposite end then the angle is not 90. Obliviously when 6x3 is adjusted to match opposite end the planes become 90. 

Why are the planes not at 90deg when the ends are at different sizes?

Im looking at this from a fabricators point of view as they would have to keep the tubing square vertical and horizontal. If i lay a pieces of square tubing alone a sketch lines I would think the surface would be horizontal and vertical to each other and origins, but this does not seem so, when modeling. 

Any comments, thank you for looking.

 

serpennica_1-1702654373158.png

 

 

 

serpennica_0-1702654157545.png

 

Message 13 of 14

Hmm. IIt's hard for me to relate.
@serpennica  This topic has been repeated many times over the last two months.
The inventor works properly and has basic knowledge of trigonometry.

 

 


If this has solved your problem, click Accept Solution.
If it helped you, click Like.

YouTube - Inventor tutorials | WWW | LinkedIn | Instagram

Message 14 of 14

Here from a different perspective:

 

 

Trigonometric functions are not linear functions.
It was, is and will be.

You are trying to force a measurement in a direction parallel to another plane.
The inventor (which is logical) understood in the direction normal to the axis of intersection of the plane.
The inventor works properly and you can work on your spatial imagination.

 


If this has solved your problem, click Accept Solution.
If it helped you, click Like.

YouTube - Inventor tutorials | WWW | LinkedIn | Instagram

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report