Help With Lofting

[Anonymous]

I am trying to loft and get a major issue when I include the top rail. I had successfully lofted without the corner rails but it created an undesirable shape in the corners, so I added rails there. Now the loft fails when I include the top rail. Does anyone know why this is the case and how to fix it? I've included a public link below.

https://a360.co/2Lqscu5

[Anonymous · Accepted solution]

I have resolved the issue. If anyone else comes along looking for help, make sure all your rails do truly intersect the curves. Draw construction lines and add constraints to make sure. That was the issue here.

[davebYYPCU]

(Your loft has 6 rails selected, and is not in error.)

Start the rail sketch, Project > Intersect the profiles.

Hide the profiles and draw the rails, connecting to the purple dots.  (There is no other way)

Might help, 

[Jaeger1787]

I have a similar problem.  I created the drawing below a couple of years ago.

I now need to create another component, with modified dimensions.

I saved the original drawing with a new file name, then modified the profiles and created new guide rails.

I can loft only one side of the drawing:

but when I try to include the other side, it goes belly up.  I notice that the left hand end of the guide rail has a purple ring.  Presumably this indicates an error, but what?  How do I correct this, when I previously had a suitable drawing albeit with different dimensions and slightly different profiles.  Also, why has the profiles broken up to create two halves where there was previously a continuous curve?

  My replacement file is attached.

Thanks for any help.

[davebYYPCU]

For some reason beyond me, the sketch 1 has a centre line and two curves meeting at top dead centre.  All three of those articles are not constrained coincident to each other (white points).  This causes Loft to create a 3rd profile, instead of adding to profile 1.

Delete the 2 arcs, and replace it with a 3 point curve.

Fix the sketch that is yellow by Manage Lost Projections.

Edit the Loft works, now.  

Blue, orange and white sketch articles produce errors like your experience and should keep you awake at night.

Might help....

[Jaeger1787]

Thanks for the reply.  Apologies for the delay in responding.  Life getting in the way of hobbies. 

The two arcs are derived from geometry in other drawings and need to mate up with other components in an assembly.  The straight lines were created to assist in aligning the two (copied) sketches onto the same planes. 

I deleted these lines and tidied up the sketches as best I can.  I note that in profile 1, there is a white circle at midpoint.  I can make this tangental, but not co-incident. 

Each time I try, i get 'Select other geometries.'  Apart from the questionable english, I assume this indicates an error - but where?

There are similar error indicators at the end of profile 2 with a straight guide rail and with profil2 and the curved guide rail.

I notice that at the ends of the curved guide rail and one of the straight rails, there are small white circles, presumably indicating the ends are not co-incident.  Try as I might I can not get these to co-incide, with either the co-incident constraint, or the manage lost projections tool.  Manage lost projections does not seem to resolve the problem.  What am I missing?

[davebYYPCU]

Purple points.

You are correct, white points (circle) are not connected to anything.  
I was not able to fix your curves, by replacing them with a single arc did work. Black point.

As nothing is dimensioned, relative to those blue arcs, should not matter.  If it does matter, add dimensions.

Another suggestion, maybe it is a 3d sketch,  try Move to Sketch Plane.

Fusion does not play well with imported geometry.

Might help…..

[Jaeger1787]

Sir.  I am getting nowhere with this drawing.   Some of the time it
reports guide rails are not joined to the arcs.  Sometimes I can select
two segments of an arc, but not the other arc, sometimes different
segments.  Now I can not select the guide rails.  See image:


If I edit the individual sketches the arcs are (as far as I can tell
co-incident and tangential.  Often I get the 'hand' icon. This does not
mean hold this which is a logical conclusion but something else - I know
not what.

How do I ensure that the rail hits the profile?  I can not find 'Manage
lost projections.'

I attach the file for version 8 of this drawing.  Please advise where
exactly I am going wrong.   What is particularly annoying is that I
created the 3D part and printed it in an earlier version. All I have
done since is to amend  the profiles and remove some un-needed entities.

Keith

[TrippyLighting]

---

@Jaeger1787 wrote:


I attach the file for version 8 of this drawing. 

---

Nothing was attached to your most recent post

[davebYYPCU]

Referring to v6 file.  Sketch order in the browser.

As said in message 5, I found sketch 1, behaving badly.  Making the intersecting three articles at top centre position.  I deleted the top two curves, and replaced those with a 3 point arc.  Made the end of the new arc, tangent to the outside curve.

Next fix, was 3rd sketch, front point of the rail, has lost the projected point that comes from sketch 2.

Next, 4th sketch, you should project the bottom line out of both sketch 1 and 2.  Hide both those sketches, now you can confirm two purple lines.  Draw lines for rails connecting to the end points. No white points on the outline.

With these fixes, the Loft works first time.

I find it best to have Chain Select turned off, in the Loft Dialogue.  
This means you build the profile selects as you need them.

Might help….

[Jaeger1787]

Thanks again for your help.  However, I am still struggling.

I have named all the sketches - something I normally try to do as I
create a design.

I have replaced the short arcs in both sketches with 3 point arcs.  I
have made these trangential to the end curves.

I have fully constrained the end profile sketch and the roof profile
sketch.

How do I get lines in one sketch (such as the curved or straight guide
rail onto the end profile?  When I draw these two sketches, they snap on
to the roof profile, but will not snap to the end profile either end or
mid-points.

I am now trying to 'project' the curved guide rail onto the end profile
at the mid-point of the arc.  I do not understand the dialogue box for
the projection tool.    I do not know if I should have the curved guide
rail, or the end profile as the active sketch.  Either way, I can select
first one, but not the other. The Help documentation does not tell you
in clear english HOW to project an entity.  If I am trying to project an
entity in one sketch to an entity in another sketch, which is the
primary sketch?

I eventually managed to link the curved guide rail to both profiles. 
The dialogue box shows Profile 2 to be connected, but in practice it
does not appear so.

When I try to surface/loft between the two profiles, I find I can not
select the smaller diameter arcs at the ends of the 'end profile' sketch.

Thanks for your help so far, but this is giving me hours of frustration.

Keith

[TrippyLighting]

Please share the design and make sure it is actually attached to the post.

[davebYYPCU]

Sent PM.

[Jaeger1787]

I actually had sent the design (by a separate message) but it appears not to have arrived.  Anyway, here it is again (hopefully).

Regards.

[Jaeger1787]

Sir.

I notice that when you select 'Edit Feature' you get the Arrow cursor.  When I do the same, I get the hand and am unable to select anything.  Unfortunately, I can not send you a screenshot.  When I try to capture the screen the hand cursor disappears.......

However, I found that I could create two new lofts by selecting the smaller arc on the roof profile, then the end profile.  That filled in one end.  I repeated that at the other end but it seems to be unnecesary by your demo, for which many thanks.  But why for you and not for me?  It is this seeming ability of Fusion to perform a task at one time, but not at another time under what should be identical conditions that is so frustrating.

Anyway, here is a screenshot showing the model after thickening.

The end profile has now been trimmed to produce a compound curve in three planes.  Many thanks for the assistance from everyone.  But, whilst my problem has a solution, I do not know where I went wrong with the surface lofting.

Lastly, what is this new icon that has popped up: 

Regards

Jaeger1787

[Jaeger1787]

It seems that I can no longer post as an accepted solution as that option is missing from the webpage, but for me, it is solved (until the next time).