Creating a Part starting from a STEP file... ?

[claudiodeviaje]

Hello again!

I have a STEP file which I downloaded from the manufacturer's website. It is just a Profile that i want to extrude.
The STEP-file wont save any features with the model and it will be handled as a solid body. Since I need to modify the part I'm trying to transform it to a PAR-file.

I did this once, but just forgot the trick. What I did was to open the Step file, then create a 2D drawing of the profile, and then created a 3D Model starting from this 2D drawing.
My problem is that after selecting "create 3D from 2D" SolidEdge won't let me select the profile

The Profile is in the "sheet1" tab and not in "2D Model" tab... does this has somethbing to do?
How do I move it to the "2D model" tab?
Would it work if I move it there?

Thank you very much!

Claudio

 

[claudiodeviaje]

If you just want to take a look at the step file, you can download it from here:
STEP File

Cheers,
Claudio

 

[donyoung]

Hi,

the named file contains a valid 3D-Body and it can't be opened
by using a .dft template.
Just do a File --> Open select the file type to be .stp
and select your file. After pressing open choose the normal.par
as template.
You should then have a valid body which you can modify. What you
do not have is a profile and all the features the part is made
of but this is the intention behind STEP

To modify it say get it to length use the direct editing capability
of SE sample
modify toolbar --> select Move face
- select the upper face, click the green checkmark
- move it upward, key in a distance
- do an LMB

that's it

SO there is no need to start with a Sketch/Profile in this
case.


dy

 

[donyoung]

/Edit

I suppose you created the draft from the 3D-Model the .stp
file does contain. I this case SE won't let you create
a 3D from that derived part -- you already have one!

The only thing you can do in this case is this ( but the View
will no longer be associated with the part!):

select the view
RMB --> convert to 2D View
OK
RMB --> Draw in View
CTRL-A (all gets selected)
CTRL-C

switch to an empty part
select sketch and chose x/y plane
select the 'Select' icon to get out of Line mode
CTRL-V

now you have a completely unconstrained sketch with a scale of 1:1

Instead of using the existing view just make a new one (top view)
which you may later on delete

dy

 

[claudiodeviaje]

Thanks for the prompt answers!

I know that the idea behind STEP is that you are not able to modify anything. But I just have to!!

I managed to do it using a similar procedure as the one described by donyoung. It was just a little longer detour...

1.- Open the STEP-File in the normal.par
2.- Create a 2D from the Part.
3.- save the drawing als DWG. If I save it as draft, SE won't let me select any lines to create a 3d Modell
4.- Open the DWG, select everything and create the 3D Modell with the Profile.

It seems that when you create a 2d drawing from a STEP file, SE realizes it is intended "not to be modified" and save this info with the file. If I save it as DWG only the geometry will be saved. All the extra info will just be deleted. When creating the 3D Modell I just have to take care, that the scale is 1:1. If not I'd get a huuuuuge monster!

Thanks again for the help...

Claudio

 

[donyoung]

Him

[...]
I know that the idea behind STEP is that you are not able to modify anything. But I just have to!!
[...]
wrong at least since SE introduced the direct editing
capability. Now you can modify a 'dump' part without
the history being available. That is close holes, move
faces, rotate faces a.s.o

[...]
It seems that when you create a 2d drawing from a STEP file, SE realizes it is intended "not to be modified" and save this info with the file.
[...]

it has nothing to do with the data coming from a step file
Any .dft which contains a part's view is not suitable
for the 2D -- 3D approach. The 2D-Model is not modifiable
as long as it is associated with the underlying part und
thus nothing of it can be selected. Therefore an imported
dwg/dxf can be used just because ther is not associated
3D-Model.

When creating your dwg or dxf create it out of Draw in View
whenever possible. This is alwaus 1:1 in SE.


dy

 

[donyoung]

Hi,

just to give you an impression what kind of modifications can
be applied to a 'dumb' part:

Modified Icem

dy

 

[donyoung]

Hi,

the simpliest way to get your sketch without dft --> dwg --> par is:

- open the converted part (.par)
- get into sketch mode
- select the top face of the model to draw on
- use 'Include' function
- from the pull down select 'Single face'
- select the face (edges will be red)
- RMB or click on the green checkmark button
get out of 'Include'
- CTRL-A
- CTRL-C

Return
Finish
Cancel

File --> Open - New -> par

- Sketch mode
- select x/y plane
- 'Select' to get out of Line mode
- CTRL-V

that's it. It's faster done than written ....

dy

 

[HDS]

Why aren't you modifying the 3D? instead of going 3D -> 2D -> 3D-> modification

 

[claudiodeviaje]

@Don. Thats preety neat. I'll try it, since it cost lots of time to take the detour.

@HDS. I tried to modify the 3D, but I couldn't. I thought that it was impossible, but seems like it can be done.

Is it possible to change some features in a dumb part?
Can you, for example, change the size of a fillet oder chamfer, or change the thread size of a hole?

Cheers!
claudio

 

[donyoung]

Hi,

you may change some, not all, features of that part. Use
the functions on the Modify-ToolBar for it. The previous
posted picture shows some modifications I've done to
the converted Step with these functions.
Also available are all the other 'normal' functions
to modify a part.

dy