Create in place problems

[Alex123]

I am trying to create a part in place. I start off with a cube. Select "Create in Place Component". When asked to select sketch plane for Base Feature I select the top surface. Now to begin my part I have to select "sketch" and pick a plane again? (which seems redundant to me because I have alredy selected a plane when it asked to select a sketch plane for Base Feature).

Here is where my problem begins. I create my part and it looks fine in the assembly orientation. I open the part I just created and it not in the same orientation. It somehow gets flipped onto a different plane.

I have tried selecting front, top and right planes to begin with and they all get flipped from the orientation of the assembly view. This is very frustating. Is it something I am doing wrong or is it a bug? Please let me know.

[Alex123]

Can anyone help me here? I'm sure Inventor 6 would act the same way so please try it and and let me know. I posted an example in Customer Files.


Again, when I draw a Part in Place, then go look at the part itself, it doesn't retain it's orientation as it was in the Assembly.

[Alex123]

In CF it is called Orientation Problem.

[Anonymous]

It should work something like.... Create Component, pick a face or plane.
The XY plane of the new part is oriented to the selected entity with Z axis
matching the face or plane normal and you should be in sketch mode on the
local XY plane unless you have changed a default setting (like "Sketch on New
Part Creation").

If you do not orient the part to the assembly (XY parallel to XY, etc.) the
coord system orientations will differ between assembly and part, but part
coordinates are constant regardless of mode.

Also, if you don't require an adaptive relationship, don't pick a face in the
assembly to define your sketch, but pick the part's XY (or whatever) plane.

....... or am I missing the point completely? 8~)

===========================

"Alex123" wrote in message
news:f14f02f.-1@WebX.maYIadrTaRb...
I am trying to create a part in place. I start off with a cube. Select "Create
in Place Component". When asked to select sketch plane for Base Feature I
select the top surface. Now to begin my part I have to select "sketch" and
pick a plane again? (which seems redundant to me because I have alredy
selected a plane when it asked to select a sketch plane for Base Feature).
Here is where my problem begins. I create my part and it looks fine in the
assembly orientation. I open the part I just created and it not in the same
orientation. It somehow gets flipped onto a different plane.
I have tried selecting front, top and right planes to begin with and they all
get flipped from the orientation of the assembly view. This is very
frustating. Is it something I am doing wrong or is it a bug? Please let me
know.

[Alex123]

You are not missing the point at all. But no matter what surfaces I pick, the part in the Assy and the same part by itself are not orientated the same. You wrote "If you do not orient the part to the assembly the coord system orientations will differ between assembly and part". This is exactly my problem!


But how did I not orient the part to the assembly? Here is what I am doing.


Create Part in Place. Select Sketch Plane. I am going to Assy Origin and picking YZ Plane. Now I must select a Sketch Plane to start my part. I am going to Part Origin and picking YZ Plane again. I did this to try to use the same exact plane.


I look at the part I just made in Assy, than I go to Part mode and it is orientated different. I am pulling my hair out.


Can you open my post and look at it or walk me thru it step by step. Something is wrong?

[Anonymous]

Hi Alex;
I had the same problem. Check out the thread called
Assembly Skewed from 3d indicator (UCS) Dated March 1 2003
in this forum.
Hope this helps. Don O

[Alex123]

Hi Acornmac,


No, this is not the problem I am having. I already knew about that problem of rotating the part. If you can open up my file under CF and look at it you will see what I mean.


When I draw the part in the context of an Assy it is not in the same orientation in Part mode.

[Anonymous]

Rotate the assembly view so you are looking more or less normal to the
assembly XY plane.

Create Component. Clear the check box on "Constrain sketch...". Pick the
nearest face of Part1 or, probably the safer bet, just drop it in space
without picking a face.

Make the new part origin planes visible and return to assembly mode.

Since the face you want Part2 to mate to is in the assembly XZ plane,
constrain the new part XZ plane flush with that face. Constrain, as wanted,
the other new part planes to Part1 making sure the plane normals (the arrow
you see when constraining) is aligned with the assembly coordinate system.

Now edit the new part and define your first sketch on the appropriate new part
origin plane, depending on whether the first feature will be normal to or
along the existing part face.

--------------

If you are constraining the new part to an irregular shape part: When you
create the new part constrain the part origin planes flush with the assembly
origin planes and create the first sketch plane (adaptive) by picking the
desired existing part face.

--------------

I have a part template that has the part coordinate system vectors from origin
sketched in. You might try that.

---------------

Hope this is what you are after and will help get you started.

==========================


"Alex123" wrote in message
news:f14f02f.3@WebX.maYIadrTaRb...
You are not missing the point at all. But no matter what surfaces I pick, the
part in the Assy and the same part by itself are not orientated the same. You
wrote "If you do not orient the part to the assembly the coord system
orientations will differ between assembly and part". This is exactly my
problem!

But how did I not orient the part to the assembly? Here is what I am doing.


Create Part in Place. Select Sketch Plane. I am going to Assy Origin and
picking YZ Plane. Now I must select a Sketch Plane to start my part. I am
going to Part Origin and picking YZ Plane again. I did this to try to use the
same exact plane.


I look at the part I just made in Assy, than I go to Part mode and it is
orientated different. I am pulling my hair out.


Can you open my post and look at it or walk me thru it step by step. Something
is wrong?

[Alex123]

Hi Jeff,


I got it to work finally. I took your advice and constrained the planes from the part to the assembly planes before I started to sketch. It seems like a lot of extra steps to Create a Part in Place but I guess this is how you do it. Thanks for your help.