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Silhouette

Phenom
Phenom

Ciao

 

In our company we use NX for CAD and Surfcam for CAM.
Now we have established that we will use NX also for CAM.
The guys who will use the new cam ask if there is a command, in NX, that in Surfcam extracts the silhouette of the workpiece, projects it onto a plane and offsets it.
Can anyone help me?


Thanks, grazie

12 REPLIES

Re: Silhouette

Gears Phenom Gears Phenom
Gears Phenom

silhouette creation :

     curves:

-isocline (asociative)

-or extract curves, silhouette , direction view, non asociative

 

You can then create plane (on such curve+offset plane)  - sketch - project silhouette curve into sketch - then  offset curve.

 

*Workpiece - probably need workpiece as a body, not the automatic shape

---------------------------------------------
#♫ PB, 5ax, itnc, nx, vericut ♫ #

Re: Silhouette

Siemens Legend Siemens Legend
Siemens Legend

You could also use the Intersection Curve, Project Curve, and Offset Curve functions to achieve what you are trying to do. These are found under the Curve tab in the Derived Curve group.

 

Capture1.JPG

 

First, use the Intersection Curve function to get the silhouette curves of the workpiece. You will need to select the outter most faces for Set 1 and a defined plane that crosses through those faces for Set 2. Note that some geometry shapes can't have all their silhouette faces intersected by a simple plane.

 

Next, use the Project Curve command to project those curve you just created to an offset plane where you want them to be. The input curves, offset plane and the projection vector will need to be defined.

 

Finally, use the Offset Curve command. In each step the created curved can be associative (automatically update when geometry changes) or non-associative.

 

In the case where a plane does not intersect with all the outside faces, the Extract Curve command can be used with the Silhouette Curves function.

 

Capture2.JPG

 

The curves derived from this can then be projected and offset as previously explained. However, note that the Extract Curves command is now hidden in NX12 since it is considered legacy functionality.

Re: Silhouette

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

What do you need the silhouette curves for?

There might be other ways without the need to use extracted curves.

Stefan Pendl, Systemmanager CAx, HAIDLMAIR GmbH
Production: NX10.0.3, VERICUT 8.1, FBM, MRL 3.1.7 | TcUA 10.1 MP7 Patch 0 (10.1.7.0) | TcVis 11.4
Development: C (ITK), .NET, Tcl/Tk Testing: NX12.0 | AWC 3.4 Preparing: NX12.0

Employees of the customers, together we are strong Smiley Wink
How to Get the Most from Your Signature in the Community
NX Customization - Best Practice Guide

Re: Silhouette

Valued Contributor
Valued Contributor

I agree with Stephan's questions.  We are curious about your programmer's work flow because they will undoubtedly approach their work pieces using different methods available in NX and could discover better and faster methods.

 

Were they using Surfcam or Surfcam Traditional?  I heard Surfcam is re-branded Edgecam and Traditional is the old Surfcam product.  The latter is light years behind most high end CAM software, in my opinion.

 

 

NX 12.0.1

Re: Silhouette

Phenom
Phenom

Ciao,

 

First of all, thank you all for the answers.

I use only the CAD and I want to help my colleagues who use only the CAM, these my colleagues make prototypes using the milling machine.
The real parts can be made with other means of production. In this case the part is made by Progressive Die.

 

sh1.png


My collegues prepare the workpiece as show below

 

sh2.pngWith surfcam they realize the ??? area with a simple passage as I explained in my first post.

To do the same thing I had to extract the silhouette curves which are not on a single plane, project them onto a plane, offset only some of them and finally connect them with some bridge curves.

 

sh3.png

If I use the projected curves as they are, the following error message appears.

 

sh4.png


So how @Mould_United says, is there a better or different way to make this with NX?

 

Ciao

Re: Silhouette

Valued Contributor
Valued Contributor

My mistake; I was under the impression you were looking for information on tool path operations...

NX 12.0.1

Re: Silhouette

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

You don't say what NX version.

Is the ability to sweep a solid finally in the product, or is it still preview project?

If available, and nothing else is suggested, you could sweep the solid, subtract from a block, then use the edge curves of the "hole" in the block? (or section the swept solid, or...).

 

But I would still ask...What are you trying to accomplish?

Could be there is an easier/different way to do it in NX without creating geometry...

Ken Akerboom Sr CAx Systems Engr, Moog, Inc.
Production: NX10.0.3.5 MP16/TC11.2
I'd rather be e-steamed than e-diseaseled


Re: Silhouette

Phenom
Phenom

@Ken_A wrote:

You don't say what NX version.

Is the ability to sweep a solid finally in the product, or is it still preview project?

If available, and nothing else is suggested, you could sweep the solid, subtract from a block, then use the edge curves of the "hole" in the block? (or section the swept solid, or...).

 

But I would still ask...What are you trying to accomplish?

Could be there is an easier/different way to do it in NX without creating geometry...


Just so @Ken_A,  I'm not a CAM user so I'm certainly making the mistake of 'blindly' following the wishes of my colleagues.

The workflow described above is the same they follow with Surfcam (old version). Probably a NX CAM user would use a different approach to do the same thing.

Maybe I did not explain myself well: what my colleagues 'pull out' of the milling machine is what you see in the second figure: yellow+gray+blue. Then they break the blu little bridge.

It is very difficult for me to explain myself: I don't know CAM and barely I write in English....

 

NX 11

 

Ciao

 

 

Re: Silhouette

Valued Contributor
Valued Contributor

Hi,

 

There seems to be a gap between your projected curves, I think thats why you have an alert.

 

gap.png

 

You may need to find and add that missing curve to projection from most outer edges of your geometry.

 

There is no automated solution for this in NX (creating geometry that lets you 'pull out' your workpiece) You need to project curves and extrude it. There might an easier way of modelling like @Ken_A described.

 

There is also no automatic way to add connecting tabs (Blue geometry). You need to model it yourself. To automate this in the future, you may use User Defined Features maybe.

 

As I understand surfcam does what users want in an automated way. But I would still insist to use NX for both CAD and CAM if I were you, for me its important to keep workflow integrated.

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