Routes not parallel

I am having this problem lately at it is going on my nerves.

I create a route and it is constrained to be orthogonal. When i move it to drawing and try to measure along cetnerlines of the pipes, it ends up that some of the lines are not parallael to each other (offset ranges from 0.00° to 0.03°) even though i do have all of the constraints to make it parallel (and at right angles).

If i want to come back to the sketch and constrain the routes at 90° it pops out the overrconstraint error (as it should) and it clearly shows angle of 90°.

What is going on here ??

SolidworksRouting
Answers 7
JB
JB 2013-10-15 Best Answer

Mladen, since this is a 3D sketch, the parallel relations aren't going to mean a lot.  Basically any two lines that cannot be projected to an intersection in 3D space can be considered parallel.  So start by deleting that relation.  You don't need the 90° dimension because your transverse pipe already has an Along X to orient it to your vertically running legs. 

Check to make sure your connection points are on the same plane as your bends.  If they are, then you can fully define your sketch with an Along Z on the right leg.

If they aren't, then get rid of the axis relations and constrain the sketch using parallel and perpendicular relations to existing sketch geoetry and planar faces.

MP
MP 2013-10-15

I have tried all possible constraints. The point I am trying to make is that in the sketcher, when you dimension the route, it is showing the lines are parallel. When moved to drawing it is showing a slight ofset. That should not happen

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PV
PV 2013-10-16

Mladen,

Instead of using 'centerlines' have you checked the actual sketch lines in the drawing, as in make the 3d sketch lines viewable and measure/check those.

The reason I mention is because centerlines can be moved independantly from the underlying model. Now while it's true that the centerlines, when newly made and if the made in the correct fashion, should be collinear with the 3d sketch the fact remains that perhaps either you're doing something wrong or the program is at fault while creating the centerlines.

Either way by checking the 3d sketch in the drawing you can narrow down what is going wrong.

MP
MP 2013-10-16

Bloody hell.. When I pick route sketch, then it gives me correct dimension.... That is weird. But I am still having problems understanding how " centerlines can be moved independently from the underlying model." is possible. That is potentialy serious problem. I created the centerlines by clicking on auto centerline the whole view. It does not make any difference if I click on pipe line one by one to create them....

PV
PV 2013-10-16

I know it's really tempting to use centerlines. It's the most natural thing to do in technical drawings and even more so in piping BUT 'centerlines' on SW drawings are purely cosmetic, as in that they don't have intelligence behind it. Nothing wrong with that as long as you keep that in mind.

When using the 'centerline' functionality you can either let it do the entire view automatically or select 2 entities (let's say the two outside wals of a pipe) and create 1 centerline.

You might not have noticed but when you change the model so that he position the pipe in question moves then the centerline on the drawing doesn't move with it.

So if the drawing that you had with the problem actual did have a small discrepancy in the model so that it wasn't perfectly parallel then when you checked and made sure that it was parallel it didn't alter the already made centerlines.

MP
MP 2013-10-16

I was aware of the things you worte in previous post, but did not take them into account...

Anyway, i think i might have found what could be the inderlying issue.. if you look at the photo below, you will see a kink in the pipe edge line...i do not know why it is that why, but probably that is the reason why there is an ofset. I will have to see my pipe model to see if everything is OK, and then backtrack all of the steps involved to find out the real cause.. thanks

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MP
MP 2013-10-16

I have unmarked correct answer as this discussion only brought me to the real reason why i was having problems. As i zoomed in on every part in my configuration, I found out following.

As you can see from the photo above, my route sketch is not going through the CPs on elbows. This is the problem, right?

I have figured out that this is happening only while i am usng my Socket-Weld fittings. I was looking throuhg it and could not find anything odd. I am attaching it, so i appreciate anyone helping me figure out this mess....

thanks

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