How to make adaptive 3D sketches?

[barnadaniel]

Hi,

I thought I know how to make adaptive parts, but it seems it doesn't always work as I believe.

I created first the rectangular part visible in the attached picture adaptive-3d-1.PNG. I have then created an assembly, and put this part into the assembly. Next I created a part within the assembly, made sure it is adaptive, edited it within the assembly, and created a 3D sketch: the spline for a sweep path. For the creation of this spline, I have used Include Geometry, and included two edges of the rectangular part. I constrained the spline endpoints to the endpoints of these lines, and made them tangent. When changing the size of the rectangular part, the swept part does not seem to follow the changes (yes, I did click on Update) - see the second picture. When editing the 3D sketch of the sweep path, I can see that the two included edges remained at their original position, i.e. they are not associative to the edges of the rectangular part. How could one do this?

Thanks

[barnadaniel]

In the meantime I figured out that one needs to use work points for this: create work points at all 4 corners of the rectangular object in my example, then in the 3D sketch, create two construction lines between 2 and 2 of these workpoint, these lines representing the edges. These can be used to for the associativity.

There must be good reasons for it, but I find it confusing that

- although one can use work points of other part files to draw lines in an adaptive 3D sketch of another part

- one can not apply constraints involving these points (for example, I would like to draw a 3D line which starts from one workpoint, and goes through another one - how can I do this?)

My workaround for this would be to create a construction line in the 3D sketch, connecting these two workpoints, then constrain my real line to be parallel to this line. Are these extra steps really necessary? Is there no better way?

Thanks

[bms953]

hi

u can use project geometry commond and u should project edge of the first part, and then use one of point in the start or end line ( project line) then u can convert project line to construction object

[bms953]

after create 2d sketch and project the edge, u cand finish sketch and create 3d sketch and use 2d sketch for create 3dsketch

[barnadaniel]

I tried, does not work. Created a part within the assembly, 'Constrain sketch plane to selected face or plane' was checked. I selected one face of the box, projected two edges, made them construction lines. Finished the sketch, created a 3D sketch, 'Include Geometry' for these two lines, then created a line connecting two endpoints.

When later changing the size of the box, the 3D sketch does not follow...

[bms953]

hi again

u don't need to include geometry in 3dsketch, after create 3dsketch can use line tool for create ur path then select one side of project line, u can use this file

[barnadaniel]

Amazing, it works, indeed. Thanks a lot. But this makes me a bit worried. The conclusion from this is that Project Geometry (in the 2D sketch environment) seems to keep associativity, and Include Geometry (in the 3D sketch environment, which I believed to be the analogue of Project Geometry) does not keep associativity. It seems I still did not get the basic philosophy or concept in Inventor, and I have the feeling that I need to memorize for each operation, one-by-one, how it works... otherwise I mess up my model - which I am actually doing permanently, due to such misunderstandings.

There is one more question: what if I want to make my spline tangent to one of these edges? I can only impose a tangent constraint between lines within the same 3D sketch, so finally I need to Include Geometry this line from the 2D sketch. But since this breaks associativity, the spline will not update to remain tangent to that edge of the solid body. Any suggestion for this?

Before your answer, I concluded myself that I need to

1 - create work points in Part1

2 - in Part2, create the 3D sketch spline anchored to these work points, because work points from another part file are available

Again, searching analogy, I believed that ALL work features of Part1 are then available in this 3D sketch of Part2, so that I can create a work axis in Part1 (anchored to an edge in Part1), and I can make my spline tangent to this work axis. But I can not, I can not even use Include Geometry for this work axis...

[barnadaniel]

I found a solution. Currently, at my level, this seems to be the best way to pass geometry information associatively between parts. Edit the part in place, then use the Copy Object operation, select the body that you want to anchor the spline to, and copy it as Composite. Then create the 3D sketch. Each edge and corner of the copied body is available for constraints, point locations, etc, associatively, no Include Geometry or Project Geometry is needed.

[bms953]

ur welcome, and i'm glad to can help u