Skip to main content
S
snguyen1-Visitor
1-Visitor
February 11, 2015
Question

Silhouette curve creation in Creo 2

  • February 11, 2015
  • 6 replies
  • 6519 views
Good morning,

I have a weird part that will have a crazy split line and
would like to create a silhouette curve of where I think the split line will
be on the surface but at the moment I do not have access to mold license. I
know in ProMold I can create it but is there a way to create it in a regular
flex engineer license?







This is the view I want the curve to fall on the part. I tried to create a
sketch and then project it to the surface but some areas of the part I
cannot use the project on some of the edges of the part.



Thanks.



Son T. Nguyen

108 W. 2nd Street

Assaria, Kansas 67416

785-667-7763



6 replies

B
bokm96061-Visitor
1-Visitor
February 11, 2015
1 copy all exterior surfs.

2 Use a surface trim operation via plane- trimming the quilt created in 1.

3 normal of the trimming plane should be coincident with your pull vector

4. i believe there is a fly-out or option to trim via silhouette

5. perform the trim.

6. create a composite datum curve on the trimmed edge of the quilt.

7. layer off the quilt....to only see the curve..





On Wed, Feb 11, 2015 at 9:33 AM, Son Nguyen <->
wrote:

> Good morning,
>
> I have a weird part that will have a crazy split line and
> would like to create a silhouette curve of where I think the split line
> will be on the surface but at the moment I do not have access to mold
> license. I know in ProMold I can create it but is there a way to create it
> in a regular flex engineer license?
>
>
>
>
>
> This is the view I want the curve to fall on the part. I tried to create a
> sketch and then project it to the surface but some areas of the part I
> cannot use the project on some of the edges of the part.
>
>
>
> Thanks.
>
>
>
> Son T. Nguyen
>
> 108 W. 2nd Street
>
> Assaria, Kansas 67416
>
> 785-667-7763
>
>
>
C
cprice1-Visitor
1-Visitor
February 11, 2015
Try placing the udf on the part. (silh_curve.gph)

This should help.

Charlie Price
Strategic Technical Services LLC
Phone 330.887.9295 Desk/Mobile/FAX
Main 888.479.1566x127
charlie.price@stechservices.com
----------
D
DonSenchuk12-Amethyst
12-Amethyst
February 11, 2015
Copy the geometry.
Paste the geometry.
Create a surface extrude where you want the parting line.
Create an intersect feature between the extruded surface and the copied geometry.
B
BobSchwerdlin1-Visitor
1-Visitor
February 11, 2015
I have also used Pete’s method in the past, with success.

Bob
S
snguyen1-VisitorAuthor
1-Visitor
February 12, 2015
Thank you for all the suggestions and I got the curve I needed with using this method recommended by Pete. I did not get a chance to try Charlie’s method. I will try that one when I get this project done.



Thanks.




B
BD_105724741-Visitor
1-Visitor
December 26, 2023

Hello,

 

You can find the silhouette trim feature in the trim command.

 

Make sure to choose a directional surface (in this case a datum plane) to use as a reference.

 

Please see the attached image.

Terms & ConditionsCookie settingsAccessibility statement