Library Features

[oneeyedwitchdoctor]

I have created a simple revolved feature, however when I insert it into a part it can only be orientated one way. I imagine that there will be an easy fix for this, but unfortunately I cannot find it. To create the library feature I used the OD of the base cylinder as a reference, then also used the end face edges as references in my sketch.

 

[JMirisola]

It probably has something to do with the sketch the feature is created from. There are different ways to deal with it...you could RMB->edit sketch plane, or edit the sketch. You could edit the library part and put in a locating sketch. Search the help files for library parts...

Jeff Mirisola, CSWP
Certified DriveWorks AE

http://designsmarter.typepad.com/jeffs_blog

Dell M90, Core2 Duo
4GB RAM
Nvidia 3500M

 

[meintsi]

The most common mistake when creating these is that the sketches are created using vertical and horizontal constraints. Always use perpendicular and parallel wherever possible.



Remember...
[navy]"If you don't use your head,[/navy]
[navy]your going to have to use your feet."[/navy]

 

[oneeyedwitchdoctor]

Here is a screen grab of my sketch to see if this can shed some more light on the matter, as I tried playing around with relations etc, to no avail. The basic crux of the matter if that the pin I am trying to make a library feature has to be able to flip depending on which side of my sketch I want it on (imagine looking at the front plane - well I might need to put it on the right hand or left hand side of the base part). My library feature parts cannot "flip" whereas ones pre-installed can ?!?!?! :-(
I think that when I choose one edge as a reference (if it is the correct one) then the sketch is cut from the material, however, if I chose the other end then the sketch is being revolved thru thin air. This is only my guess so any other ideas are appreciated.

 

[CorBlimeyLimey]

That file was created in a newer version of Word than I have. Can you repost just a simple screenshot (jpg, bmp, etc) without using Word? The actual SW file would be even better.

 

[oneeyedwitchdoctor]

As requested, here is the SW file

 

[mncad]

oneeyed,

Check this thread559-191263, as meintsi suggested, try to eliminate all refernces to horizontal, vertical, even the origin and planes, the less the better.

mncad

 

[CorBlimeyLimey]

I think that one of the problems is that a Library Feature (LF) cannot include the base (first) feature if it is to be added to another part which already has a base feature of its own. Yours appears to include the base feature it was created from.

 

[meintsi]

As nmcad said above, less is better and looking at your file your are over constrained.

Loose the second edge reference and replace with a dimension. Then it should be able to flip.

Also remove the two fillets and re-add them as sketch fillets for a variety of reasons.

Remember...
[navy]"If you don't use your head,[/navy]
[navy]your going to have to use your feet."[/navy]

 

[oneeyedwitchdoctor]

Thanks very much for all ur help on this matter. I have managed to get this and other librarys features working as planned now

 

[CorBlimeyLimey]

So what was the solution(s) to making the LFs useable?