Detached centre lines in drafts

[Raaden]

Ok so this is the case:

I have placed "Centre line By 2 lines" in draw in view in the draft.
Made some changes in the part file and saved.
Update views in draft
And of course the result becomes:"Annotation (center line) detached"

So my question is: Has someone found a way to reattach the center line after this? This is really annoying when you have many "symmetric diameter" dimensions that uses this particular center line as base.

Thanks

 

[KENAT]

Re-attaching the cl is easy if I've understood your post.

From memory:

When you select the detatched line you should see 2 black squares at each end.

Simply drag the inner square with the left mouse button to the point it should be attatched to and if you get it close engough it should snap to it.

Hope this helps,

Ken

 

[SLemin]

AFAIK, you have to hold the ALT key down while dragging, then it'll reattach to the part

 

[fredericmenage]

Hi,

There will be 4 black squares. Take the ones that are not at the extremities and just drag them to the middle (go approximately because the midpoint indicator will not show).

It should reattach easily. When it is attached, the geometry it attaches to should be highlighted.

NB: no need for 'ALT' when reattaching something that is detached.

Fred

 

[beachcomber]

Try not to use centre lines for dimensions - use the FEATURE edges instead.
For example, click the circle edges or centre point to place hole centre dimensions.
For symmetric diameters you can select the mid-point of the edge representing the nd of the cylinder as the origin point.

I've tried the solutions above but you can't re-attach it as 'between 2 lines' - it always goes '2-points', so take care that it's the points you want.

Another way is to 'draw in view' and constrain a centre line to the view, rather than using centre line command.

bc

 

[Schipperus]

I think his problem is a little more complex. When a centerline cannot be placed by two POINTS (because it doesn't end on a snappoint on one end, or both ends), you will have to place it by two LINES. When reattaching the centerline, holding ALT the only reattachable points are the endpoints, which you cannot attach, because the is no snappoint to attach to.

I have had this problem several times, and I haven't found a solution to this.

IJsbrand

 

[Raaden]

Thx for the answers guys.

It is like Schipperus wrote; you can reattach the center line against 2 elements but snappoints are unavailable and placing it by freehand is really not an option here.

I did find a quickfix for this though, on my cylindrical bonnet I drew 2 small lines at the midpoints where I would like to place my center line like this:
____________
| | Btw the square is a pipe,
-| |- too hard to draw a bonnet in ASCII
|____________|

Then I just reattached the center line to the drawn lines and everything was just fine and dandy again.

And beachcomber; I usually make my center lines in "draw in view" with the line command and think that it's the best way really, but this time I did a copy-modify job and hadn't made the original drawing.
I don't agreee with you on the feature edges part though if I have drawn the center line with the line command I always use that one as base for my symmetric diameters.

I forgot to say that I run SE V16 in my first post, but I don't know if it really matters.

/Pontus

 

[donyoung]

Hi,

in V16 you have to use the ALT key (Schipperus wrote)

Assuming the center line was placed with the function
centerline by 2 lines (your picture):

pick the inner square and just move it anywhere to the top line
(the line gets red)
then pick the other inner square and move it anywhere to the
bottom line

the center line should snap to the midpoints of both the right
and left edge

dy

 

[Raaden]

Hmmm, guess I was real tired last night, the center line I had problem with was originally made with the "by 2 points" placement option, a "by 2 lines" center line would be reattached just like donyoung wrote.

So I guess that the problem still stands, but now for a "by 2 points" line.

 

[donyoung]

Raaden,

with 2 points it will work as described in V18.
To reattach you only need to grab the connecting point(s)
with the LMB and move them (for 2 lines this should work
in V16 too). With V18 the ALT key must be used when a
different element/point is to be assigned.

dy

 

[Raaden]

Ok I haven't tried V18 or 19 yet, but hopefully we will upgrade early next year and hopefully my problem will disappear. Thanks Don

 

[donyoung]

Raaden,

hopefully, but be warned the problem with detached centerlines
is still around. So when ever possible avoid to use them for
dimensioning.

dy

 

[KENAT]

I never used to use the centerline command because of this problem.

However, I've noticed in V17 & 18 it's a lot better. Still sometimes fails but less often and seems easier to correct.

I used to draw all centerlines 'draw in view' with the line command and not even use the center line command.

Even so I rarely if ever dimension to the CL however I've created it, I try to use actual model geometry.