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: 

Bend part doesn't work with thread feature present

17 REPLIES 17
SOLVED
Reply
Message 1 of 18
-niels-
1631 Views, 17 Replies

Bend part doesn't work with thread feature present

I've attached an example of a workflow we use to make different instances of products.

part1 gets assembled in assembly1 which then gets derived in part2 to receive a bend.

We use assembly1 in one place and part2 in another.

(this is a simplified example, made with IV2013 SP1.1)

 

Now for the problem:

In part1, if you add the thread feature, the "bend part" feature in part2 fails after updating.

This also happens if you try to add a "bend part" to part1 AFTER the thread feature, if the bend is present beforehand it does work.

Having the bend before the thread feature in part1 doesn't work with our workflow, because we need the assembly1 to be straight.

 

In short, the thread feature is causing problems with "bend part".

 

I can't say if this problem was present in previous versions or even in the previous service pack since we don't use this workflow that often, especially with threaded parts, but i hope this can get fixed with a hotfix.


Niels van der Veer
Inventor professional user & 3DS Max enthusiast
Vault professional user/manager
The Netherlands

17 REPLIES 17
Message 2 of 18
JDMather
in reply to: -niels-

I don't see a Bend Part feature?

I don't see a sketch for adding Bend Part feature?

I don't see derived part?


-----------------------------------------------------------------------------------------
Autodesk Inventor 2019 Certified Professional
Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional


The CADWhisperer YouTube Channel


EESignature

Message 3 of 18
-niels-
in reply to: JDMather

The bend part feature should be present in part2, so you don't have to add it yourself.

Part2 also holds the derived assembly1.

Part1 should have a thread feature under the EoP which, when included, should show the error in part2.

 

Maybe the way i wrote it caused confusion, if so i apologize, or is there something missing in my attached files?

 


Niels van der Veer
Inventor professional user & 3DS Max enthusiast
Vault professional user/manager
The Netherlands

Message 4 of 18
rdyson
in reply to: -niels-

Strange indeed!

(JD you need to open part2, it's not included in the assembly)



PDSU 2016
Message 5 of 18
JDMather
in reply to: rdyson

My mistake, I saw the two parts in the assembly and did not look close enough to see that it was too instances of the same part.  Never opened  Part2.

 

I did some experimenting creating the geometry in a single part and it failed as well.


-----------------------------------------------------------------------------------------
Autodesk Inventor 2019 Certified Professional
Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional


The CADWhisperer YouTube Channel


EESignature

Message 6 of 18
-niels-
in reply to: JDMather

JD, Rdyson; do you happen to know if this problem was present in previous releases of IV?

I'm just wondering if this ever worked or not...


Niels van der Veer
Inventor professional user & 3DS Max enthusiast
Vault professional user/manager
The Netherlands

Message 7 of 18
rdyson
in reply to: -niels-

Sorry, no idea and and only go back to 2012.

Here's a work around, until someone from Adesk pops around (maybe).

I used the thread modeler plugin from Labs.

Not ideal but might work for you.



PDSU 2016
Message 8 of 18
-niels-
in reply to: rdyson

I must say that your proposed workaround looks really nice!

But, sadly, by modeling the thread you can't use the thread/hole note annotation on drawings, so I can't use it in our situation. Smiley Sad

I wouldn't mind getting a link to that plugin though...

 

 


Niels van der Veer
Inventor professional user & 3DS Max enthusiast
Vault professional user/manager
The Netherlands

Message 9 of 18
rdyson
in reply to: -niels-

If you unsupress the thread feature, hole note works in the drawing. Unfortunately that will also cause the bend to fail, so not a solution.

The plugin has been move to Autodesk Exchange Apps.



PDSU 2016
Message 10 of 18
jakefowler
in reply to: rdyson

Hi niels,

 

Many thanks for posting this issue, and apologies for not responding to this sooner!

 

I've taken a look at our problem database, and this doesn't appear to be an issue we've seen before. I've logged this as issue 1478607 and assigned this to the development team, so hopefully we can look into getting this fixed for a future release.

 

The problem only appears to affect non-Full Length threads, so an alternative workaround I can offer for this model is to split the part face at the point where the thread should terminate, and then perform a Full Length thread on the split face (see attachment). This allows the Bend to compute successfully, and this should also allow you to annotate the drawing correctly.

 

If this doesn't work for your workflow, let me more details and I'll try to offer further assistance.

 

Thanks!

Jake



Jake Fowler
Principal Experience Designer
Fusion 360
Autodesk

Message 11 of 18
-niels-
in reply to: jakefowler

Hi Jake,

 

Your workaround works perfect for us, thank you for that.

I still hope the issue will get fixed, but at least now we can move on.

 

Regards,

Niels


Niels van der Veer
Inventor professional user & 3DS Max enthusiast
Vault professional user/manager
The Netherlands

Message 12 of 18
JDMather
in reply to: jakefowler

Good job on coming up with that solution Jake.


-----------------------------------------------------------------------------------------
Autodesk Inventor 2019 Certified Professional
Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional


The CADWhisperer YouTube Channel


EESignature

Message 13 of 18
jakefowler
in reply to: -niels-

No problem, just glad to hear that it's a workable solution!

 

Obviously we will still look into fixing your original problem, and issues in our database that come from Discussion Group posts are highlighted so that they receive special attention and priority.

 

Thanks again for posting this issue!

Jake



Jake Fowler
Principal Experience Designer
Fusion 360
Autodesk

Message 14 of 18
-niels-
in reply to: jakefowler

@jakefowler this is an old thread, but i've run across this again in IV2016. (similar issue in any case)

 

2017-02-23_1658.png

 

See the attached file, it's just a simple cylinder shape with (full) threading applied to it.

It will bend without the thread, but fails if it's enabled.

Is this still on the list to be fixed?

The workaround in proposed here with the split faces isn't applicable in this case and i would really like a way to achieve this bend.


Niels van der Veer
Inventor professional user & 3DS Max enthusiast
Vault professional user/manager
The Netherlands

Message 15 of 18
johnsonshiue
in reply to: -niels-

Hi Niels,

 

I could be wrong but I suspect this is blocked intentionally to avoid deviating thread spec. I take a look at the part and get back to you.

Many thanks!

 



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Message 16 of 18
-niels-
in reply to: johnsonshiue

Hi @johnsonshiue, thanks for taking a look!

 

Not sure what would deviate the thread; if (in the attached part) i move the thread below EoP, then apply the bend and move the EoP back the thread gets applied as in the following screenshot:

2017-02-24_0851.png

As you can see, on the idw the hole&thread note works properly on both ends.

 

The problem is that i can't use this workflow since i'm actually deriving a threaded item into another part for bending.

(hence the similar situation)

 

Eagerly awaiting your reply,


Niels van der Veer
Inventor professional user & 3DS Max enthusiast
Vault professional user/manager
The Netherlands

Message 17 of 18
-niels-
in reply to: -niels-

Update: i managed to create a workaround with the EoP method in my previous post.

It involved deleting the threaded surface with "delete face" and patching it up so i could apply the bend.

See the attached file, i hope it works with the suppressed link to the derived part.

 

It's a pretty ugly workaround but at least i can finish this now.

If there is a "prettier" solution, i'd love to see it.


Niels van der Veer
Inventor professional user & 3DS Max enthusiast
Vault professional user/manager
The Netherlands

Message 18 of 18
johnsonshiue
in reply to: -niels-

Hi Niels,

 

There are other ways to do it but nothing is straight forward or elegant. The fundamental issue here is that the thread cannot be bent. There is just no way around it because Inventor does not allow threaded face to deform and change its spec. This might be an interesting idea for Inventor Ideas.

Many thanks!



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer

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

Post to forums  

Autodesk Design & Make Report