SLDDRW: Constrain Centerlines/ Sectionlines to Temporary Axes

[wesman33]

Hey gang.

I'm running 2004 , SP2.1.

I am generating a drawing of a cylindrical part. I have not previously had much luck selecting the the end of the temporary axis to accurately position the centerlines. So my workaround to place my centerlines is to insert a point onto the temporary axis, which auto-constrains, then constrain my lines to the point.

My problem is that I have an "old guard" type guy reviewing this drawing and the extra 'x' from my point is causing him to lose sleep at night.

Any ideas on how I can do this without the point?

Thanks
-wes

PS: I can't delete the point after the fact, because then I lose the constraints on the lines.

 

[mncad]

Wesman,

We use the symmetric relation to position the center line. Just draw the centerline then pick it and the 2 silhouette edges of the cylinder and the symmetric relation.

mncad

 

[wesman33]

I should have been more specific. I was talking about the end view.

The side view I can constrain directly to the temporary axis, then hide the temporary axes.

 

[mncad]

In that case draw the centerline, use the "Select Midpoint" for the middle of the centerline, then pick the diameter of your cylinder and relate them concentric.

mncad

 

[CorBlimeyLimey]

Why are you drawing centrelines?
SW has a Centreline & Centre Mark icon in the Annotations toolbar.

Simply select the icon then the cylindrical face or circle.

from (the City of) Barrie, Ontario.

Everyone has a photographic memory. Some just don't have film.

 

[mncad]

CorBlimeyLimey,

We still draw centerlines because of the configuration of our parts. We will have a feature that is only on 1 side of the centerline but needs to be dimensioned as a diameter. If you use the Annotation Centerline you can't convert the dimension to diameter. I also use the same method for a section line thru center of the part.

mncad

 

[Dennyd]

mncad,

It sounds as though you adding the dimensions in the drawing manually. Have you tried bringing in the dimensions from the part file? You'd then be able to dimension the part the way you want and you'd still be able to use the annotation centerlines.

- - -Dennyd

 

[TheTick]

I have just examined a couple of my drawings that use hole axes to constrain section lines in drawings. No such problems in either the down-axis view or side view cases.

Are you trying to constrain a center mark or a sketched line? Can you constrain a regular sketched line?

Due to illness, the part of The Tick will be played by... The Tick.

http://www.EsoxRepublic.com

 

[CorBlimeyLimey]

wesman33
Have the above responses helped?

mncad
If you want to force the Diameter (Ø) symbol to a dimension, hold down the Alt key & type 0216 before the dimension (in the dialogue box) ie. Alt+0216<DIM> or type <MOD-DIAM><DIM>

TheTick
Yes, you can constrain sketch entities in a drawing.

from (the City of) Barrie, Ontario.

Everyone has a photographic memory. Some just don't have film.

 

[TheTick]

Cory...

I'm asking wesman if he is able to do it. Me, I've been doing it for years.

 

[CorBlimeyLimey]

TheTick
Sorry about that, I took it as an open-to-all question. I did think it strange that you would ask that type of question though ..... I'll be OK after another cup or two of ... I hope.

from (the City of) Barrie, Ontario.

Everyone has a photographic memory. Some just don't have film.

 

[Ataloss]

If you just want to hide the point, move the point to a new layer, then hide that layer. Your line will still be constrained to the point, but the point won't show up in a plot.

Bob

 

[wesman33]

Sorry for the delay, I have had, in no particular order, a French class, internet fiber line cut, and a Doctor's appointment.

Tick -
1. Cannot constrain a sketched line.
2. Cannot constrain a section line.

A different (better?) description of the situation: I am unable to constrain a section line to the center of a circle. This circle happens to be the end view of a cylindrical part, so I was trying to constrain the line segment for my section to the temporary axis of my part. When I edit the sketch for the section line, I cannot select the endpoint of the temporary axis, therefore I cannot create a constraint.

You mentioned constraining to a hole axis, my part is actually a revolved part. Would this make any difference?

 

[CorBlimeyLimey]

wesman33
A Temporary Axis does not have end points!!!

In a side view you should be able to create a Colinear constraint between your section line & the Axis.

Also, assuming you have drawn your cylinder around the part origin & planes, then in an end view you should be able to use the origin or a plane to constrain to. You can make your origins visible from the View dropdown or select them & the planes from the View Manager.

from (the City of) Barrie, Ontario.

Everyone has a photographic memory. Some just don't have film.

 

[TheTick]

In a drawing or sketch, an axis (temporary or feature) will appear as a point if it is normal to the sketch/drawing plane. It will behave like a point w.r.t. sketch constraints.

The catch is that the axis must be exactly normal to the sketch plane. SW will signal this condition by showing the axis as a point (star/asterisk like symbol) If not, it will behave like a line segment with no endpoints.

Two things to check:
1.) Make sure your line segment belongs to the view. Give the view a little nudge and see if the line moves with it. Use "Lock View focus" when sketching to ensure that lines belong to views as expected.

2.) Double-check that the axes are indeed normal to the drawing plane. Inspect the model and drawing carefully.

Due to illness, the part of The Tick will be played by... The Tick.

http://www.EsoxRepublic.com

 

[wesman33]

It looks like Lock View did the trick.

But, I still had problems selecting the center point after one line was constrained to it. After a little experimenting, I discovered a neat feature.

I moved both my horizontal centerline and my vertical sketch line (for the section line) away from the center point. I then selected the point, and both lines. After all three were selected, I was able to apply a midpoint relation and everything snapped into place.

Thanks to everyone for their quick response.

I have had much worse experiences with paid software vendor support lines. (Not SW)

-wesman