adaptive

[mortada1998]

Hi everyone 

May I know the cause of this problem, I watched dozens of educational videos on YouTube and applied what they did step by step, but it never worked for me

I use inventor professional 2020 

I am attaching a link to a YouTube video explaining the problem

https://youtu.be/_9i1EVkYDQY

[bradeneuropeArthur]

What does not work for you?

[bradeneuropeArthur]

this will explain better:

https://www.youtube.com/watch?v=bM2LksrQJ9U

[johnsonshiue]

Hi! Please share the iam and ipt files.

Many thanks!

[TheCADWhisperer]

No parts?

[mortada1998]

 

[johnsonshiue · Accepted solution]

Hi! This can be done relatively easily. I suspect either the tutorial was wrong or you did not follow the steps correctly.

Here is what you need to do.

1) Edit 12:1 in place.

2) Make Sketch 1 visible. Edit the sketch.

3) Change the vertical dimension 50mm to driven dimension. This is the key step. Without changing it, the adaptive does not do anything.

4) Finish editing the sketch -> Edit the Coil -> change the Height to d13 (or select the driven dimension). This is another key step. Without it, the coil will not change height.

5) Edit Sketch2 -> change the 50mm to d13.

6) Return to top. Edit Mate4 constraint and reselect the Workpoint1 from 12:1 as the second selection.

Please take a look at attached file. Also, watch the tutorial again and see where you missed.

Many thanks!

[mortada1998]

Thank you very much, Engineer Johnson Shiue, for this very useful clarification ❤️❤️❤️

[will.astill]

I'm trying to understand why I'm having so much difficulty using Adaptivity so I thought I'd make a very simple part and film my workflow to see what I'm doing wrong.

I think there is some behaviour that I would consider "buggy" and other behaviour that seems weird to me.

I can do this stuff in Solidworks really easily and it seems crazy how unreliable it is in Inventor.

I created a simple back plate, with a top and a bottom using two very slightly different workflows.

• Workflow 1 When creating the "Top" part I didn't click the "Constrain sketch plane to selected face or plane" option (01:30).
• Workflow 2 When creating the "Bottom" part I did click the "Constrain sketch plane to selected face or plane" option (02:38).

The "buggy" behaviour seems to be that Inventor creates either one "Flush" mate (3:42) using workflow 1 and two conflicting "Flush" mates (3:38) using workflow 2.

I had a quick go at manually sorting the issue by deleting one of the mates on the bottom part but just ended up breaking everything. I need to dig into this a bit more.

The "weird" behaviour is in the way that sketch constraints seem to be applied.
I made all the parts using what I'd consider to be good practice. In the "Top" part, I even manually added all the constraints so that I knew exactly what was there (1:55 to 2:25).

However, when I then edit the size of the "back" part (3:50 to 4:00), everything fails and Inventor complains that cross part associations have failed.
Inspecting the "top" part sketch (5:38) reveals that this is because Inventor has applied the most mental constraints possible for the projected geometry (see image below).

Can someone tell me what I'm doing wrong please? Or is this a bug in the way Inventor behaves that needs fixing?

[TheCADWhisperer]

@will.astill 

Can you Attach your assembly here?

[will.astill]

Here you go.

I rebuilt them so that they are as per 3:44 in the video.

Will

[will.astill]

...

[Anonymous]

Hi, watching the recording (plus picture, yes), and picking the assembly apart, it is clear that the reference loop was broken. To fix this, I've added a screenshot with steps and added text. Hope this helps you.

See the attachment in which I've recorded a newly created assembly (2024). Cheers, Marco

[will.astill]

Thanks for the comprehensive reply @Anonymous 

I understand that the issue is with the sketch in the "Top" feature and that it is grounding itself to the part origin. What I'm trying to work out is why this happens given that I'm following what I'd think of as a good workflow for creating the part.

I don't really want to turn off origin projection in sketches as I generally constrain parts to the origin (when not creating adaptive parts). It would be more of a pain projecting the origin in every part than deleting it in adaptive parts.

However, you got me thinking... why is the part origin projected in the top corner like that? I certainly don't want it there. It should be in the middle to match the sketch planes in the parent assembly file.

So I played around a bit and I found that the crucial step is when I follow the instruction to "Select sketch plane for base feature" (0:11 and 1:32 in the attached video).

• If I select the YZ Plane then the part origin is created where I expect it to be (0:25)
• If I select the Top Face then the part origin is created in the corner of the selected face (1:41)

So I suppose that this answers what I'm doing wrong in the workflow that is creating the "Weird" behaviour. It seems very repeatable so I need to train myself to use an assembly sketch plane to create adaptive parts.

I just need to figure out the "buggy" behaviour now.

Thanks again for pointing me in the right direction. 

[Anonymous · Accepted solution]

You're welcome, Will. I've gone back to the assembly with the broken loops and actually fixed it. The projected geometry was deleted and new lines were projected onto the sketch. The .mp4 attached shows that fix, including the modeling process.

For good measure, I've added all files to a zip folder. It includes your Inventor files, my newly created version of your assembly, plus the .png and all .mp4 files. Please note all Inventor files were saved on an Inventor 2024 version, as I don't really work with my old copy anymore (2017). Cheers, Marco