Sketch copy-extrude misalignment

thomas_holford

This is in reference to document: Octagonal Pedestal - multipart

https://cad.onshape.com/documents/28044d76fae64781bc7c9c46/w/f0b392a79f784531824bf25d/e/a228e5092b0f420ea9f87336

In Part Studio 1 of the reference document, I created a multi part sketch and extruded two types of parts in separate extrude operations.

I then copied and offset the plane of the sketch (Top Plane) creating Plane 1. Then I copied Sketch 1 and pasted it on Plane 1, creating Sketch 2.

When I selected and extruded corresponding parts in Sketch 2 to duplicate the parts created in Extrude 2, the newly created parts are slightly mis-aliigned with the Extrude 2 parts, and there is a visible gap between the Extrude 3 parts and the Extrude 1 "stringers".

I would have expected that the technique I used would have translated the parts in perfect alignment.  Am I expecting to much or is there a flaw in the technique or a bug in the software?

Narayan_K

You can do one work around, create new sketch in parallel plane created and by the help of "Use" command you can project it. for quick and easy selection after selecting "use" click on sketch1 from model tree it will project all entity to of sketch1 to new plane.

nav

thomas_holford said:

Yes.  The mirror technique would do what I want and is probably a bit more intuitive than "use".

Ultimately, I want to have three or four rings, and I suppose that the better way would be to create multiple planes and use the "use" command.

If you need multiple rings in parallel planes use the Linear pattern command.

andrew_troup

 @thomas_holford
It's very tedious and exacting to try and build such a sketch by putting down all the elements and then constraining them at the end: it's much preferable to constrain as you go, to the point that the entities (and their endpoints) go black. Unless you give enough information at the time they are created, they will stay blue (under-constrained) . If you provide the same information two different ways, they will become over-constrained, and this also should be rectified at the time it occurs.

I would recommend sketching only one rectangle, fully constrain it, then use "circular pattern" on the rectangle, then constrain the centre point of that pattern. Then you can create a single connection between two adjacent rectangles using tangent arcs and lines, and fully constrain that, finally adding another circular pattern, and constraining that centre point.

This should produce a well-behaved, fully constrained sketch with minimum effort and confusion.

Narayan_K

thomas_holford , Whenever you copy and paste the sketch it will not comes as per your original sketch position.It maintains the profile not the position.
Whenever you paste the sketch,It will matches sketch center to origin. 

thomas_holford

Narayan_K said:

thomas_holford , Whenever you copy and paste the sketch it will not comes as per your original sketch position.It maintains the profile not the position.
Whenever you paste the sketch,It will matches sketch center to origin. 

Is there a technique for precisely aligning identical sketches on parallel planes?

Narayan_K

You can do one work around, create new sketch in parallel plane created and by the help of "Use" command you can project it. for quick and easy selection after selecting "use" click on sketch1 from model tree it will project all entity to of sketch1 to new plane.

thomas_holford

Narayan_K said:

You can do one work around, create new sketch in parallel plane created and by the help of "Use" command you can project it. for quick and easy selection after selecting "use" click on sketch1 from model tree it will project all entity to of sketch1 to new plane.

Thank you.  It worked beautifully.

It's not very intuitive unless a person has some awareness and experience with the "use" command.

Another question: it looks like the "use" command will allow a sketch to be projected on a plane that is not parallel.  What techniques can be used for positioning or rotating a projected sketch on the new plane?

nav

A different workflow for what you are trying to accomplish is not to draw at all the sketch in the parallel plane but use the mirror feature instead.

thomas_holford

Yes.  The mirror technique would do what I want and is probably a bit more intuitive than "use".

Ultimately, I want to have three or four rings, and I suppose that the better way would be to create multiple planes and use the "use" command.

nav

Also @thomas_holford your sketch 1 is all blue meaning is under constrained (https://cad.onshape.com/help/#troubleshooting.htm?Highlight=red), when you copy and paste a sketch you can position it accurately using constraints, in the case of your sketch as not being fully constrained this is what happens:

Narayan_K

You can constrain all sketch entity of sketch1 such that if we drag one point or line, profile should not be altered .so that after copying the sketch we can drag the sketch and constrain it with respect to  any point.

nav

thomas_holford said:

Yes.  The mirror technique would do what I want and is probably a bit more intuitive than "use".

Ultimately, I want to have three or four rings, and I suppose that the better way would be to create multiple planes and use the "use" command.

If you need multiple rings in parallel planes use the Linear pattern command.

thomas_holford

Narayan_K said:

You can constrain all sketch entity of sketch1 such that if we drag one point or line, profile should not be altered .so that after copying the sketch we can drag the sketch and constrain it with respect to  any point.

Sketch1 appears to be constrained in many ways.  What additional constraint needs to be added to make the sketch fully defined?

thomas_holford

Narayan_K said:

You can constrain all sketch entity of sketch1 such that if we drag one point or line, profile should not be altered .so that after copying the sketch we can drag the sketch and constrain it with respect to  any point.

Sketch1 is constrained in many ways.  What additional constraints are need to fully define the sketch?

andrew_troup

 @thomas_holford
It's very tedious and exacting to try and build such a sketch by putting down all the elements and then constraining them at the end: it's much preferable to constrain as you go, to the point that the entities (and their endpoints) go black. Unless you give enough information at the time they are created, they will stay blue (under-constrained) . If you provide the same information two different ways, they will become over-constrained, and this also should be rectified at the time it occurs.

I would recommend sketching only one rectangle, fully constrain it, then use "circular pattern" on the rectangle, then constrain the centre point of that pattern. Then you can create a single connection between two adjacent rectangles using tangent arcs and lines, and fully constrain that, finally adding another circular pattern, and constraining that centre point.

This should produce a well-behaved, fully constrained sketch with minimum effort and confusion.