problem in updating a part in assembly. 1

[amitkulk]

Dear all,

i am facing one problem in assembly. I have created one assembly of two parts 1. box with a hole and 2. Shaft

but for creating a shaft i have used a edge of the hole in the box. but when i modify the hole(the dia) in the box the shaft is not getting modifed accordingly. Can any one help me with this.
Also in the shaft sketch the circle used from the box is assosiative so i am not able to give any dimension to it. I can isolate that and use it. but why its not updating in first case..

please help me in this

Amit

 

[eklunja]

Have you updated shaft's part after modifying the hole?

 

[amitkulk]

ofcourse yes

but its not updating

amit

 

[ajguerini]

Did i recreate what you are trying to do?

I created a box with a hole in it 20mm
I created a shaft with a dia of 10mm
I assembled the shaft into the hole
I clicked on the shaft in the assembly to modify
I erased the 10 mm dia dimension
redimensioned the shaft in relation to the hole with a 2 mm gap
all updated correctly (20 mm hole and 16 mm shaft)
I changed the gap to 1 mm and all updated correctly (20 mm hole 18 mm shaft)
I created a drawing of shaft and dimension is correct and updates correctly when I chang gap between hole and shaft

I amusing v5 r7

Is this what you are trying to do?

 

Hi,

I think the solution is to create another circle (sketch of the shaft) in the plan you want and then to make the dia of this circle equal to the dia of the circle of the hole by editing a formula (right click on the value field of the dia of the circle of the shaft)

Regards

G A

 

[amitkulk]

DEAR ALL,
following steps i have done

1. i created a box with a hole dia 20

2. then i created a shaft but for shaft sketch i have projected the edge of the hole of part 1.

3. after this when i modified the hole of the part1 the shaft should also be modified but it is not the result.

thats what i have done

I know that i can create one sketch and do the relations with some dimension but if the sketch would have been very complicated then it increases the time required to constrain. So i was insisting on projecting the edge.

Even one more thing i have observed if in the step 2 insted of edge the suface is projected then the shaft updates. what is the reason i cant understand...

anyways thanks for the help

Amit

 

Hi All

Amit,

Have you checked that the option that allows you to keep link to a geometry in another part in on ( under tools/options/part design) ?

 

[eklunja]

Hello,

Easy way to check wheater keep link is active on not...

Does projected line go to Open Body?
If so, then there is no link with hole and shaft sketch.

If projected line goes to External reference you have
the option set correct.

 

[amitkulk]

Dear all,

Actually the projected edge is one sketch and not in open body and it has the link. When i try o dimension the same it says its over constraint so it has a link.

thanks for the help
Amit

 

[itsmyjob]

Hi

go in Tools/Options/Mechanical...

And look for the update lines... check Synchronize before update... This means the links synch will be check before update...

If everything else is good; this should work.

Hqve fun

eric

 

[ravig]

Hi,

go in Tools/Options/Mechanical/Part Design...

And look for the General- External References,
check -keep link with selected object.
This means it will create a group with externally
referenced objects.
this should work.

cheers
Rav

 

[amitsing]

hey amitkulk
do not mention as projected line...some of the people are confused ....that is in open body (project line)...this is "use edge" what you are talking about,so it does not come in open body and has link since it cannot be dimensioned..also there is no mathematical uncertainity or computational resistance to provide a link so makers of software should have provided the link but we are not able to detect it, might be be because of some bugs.
cheers
amitsing

 

[amitsing]

hi guys and amitkulk
got it !!! u go to tools->options->assembly and then pick constraints ..u select "keep link with the selected object" ...after this do the operation which amitkulk says and then the part will be updated...this is an assembly feature and hence u have to pick up assembly under options....
cheers
amit