Bolt connection pattern: It doesn´t make the holes

[omtb]

Pattering a bolt connection, it doesn´t makes the holes only the bolt. You would expecto to build the complete connection you did( bolt ,nut , hole ....) but it does only the connecdtion , not the hole.
Is there a patch fot this? I´m using Inventor 2010 ,223b.
pleas help ,this is a basic function that inventor should do easily

[Anonymous]

Hello,

I assume you are using component pattern in the assembly. This is currently
functional limitation as new instances of Bolted Connection are simply
regular assemblies. For now, I recommend to use "Follow pattern" option
within Bolted Connection panel (See the picture enclosed). You simply need
to create hole pattern with one 'plate' and select that patterned hole while
placement is "By Hole" or "Concentric". It recoginzes the pattern
automatically and drills all corresponding holes in other components too.

Thank you for understanding. Best Regards, Ales Ricar


wrote in message news:6328206@discussion.autodesk.com...
Pattering a bolt connection, it doesn´t makes the holes only the bolt. You
would expecto to build the complete connection you did( bolt ,nut , hole
....) but it does only the connecdtion , not the hole.
Is there a patch fot this? I´m using Inventor 2010 ,223b.
pleas help ,this is a basic function that inventor should do easily

[barnadaniel]

Hi,
Following your advice, I tried the following:
1) Created a sketch within the assembly, with a circular pattern of points
2) Made 'Through all' holes at these points (btw these holes do not appear in the part files, only in the assembly)
3) Made a Bolted Connection, selected 'By Hole'. However, the 'Follow Pattern' checkbox is inactive, I can not select it. I can only select one single hole from the pattern

Tried the following as well:
1) Created a sketch in the assembly as a part (Assemble>>Create)
2) Created a circular pattern of points
3) Made a bolted connection 'On point', and selected these points (after selecting the first, the 'Placement' jumps to the 'Termination' selector, so one has to click again the arrow at the left of 'Point(s)' )

However, in this case the bolted connections loose associativity to the sketch, one can modify or even delete the sketch, the bolted connections do not change place

[awpylant42]

(I am replying just for future viewers since this was years ago.)

You have to create the a pattern of holes on one of your parts, not just a sketch, and it will pick up the pattern in the bolted connection dialog box. When you select follow pattern it will then create a set of holes through both parts following the pattern.

[engfcavalcanti]

I´m using Inventor 2018 professional and this caracteristic still remain like 2010  version. The only way is to make a pattern of the roles first.