Swept cut option

[amitpaul713]

Hi,

Can anyone help me with Swept cut option in UG? I know there is no swept cut option but is there any way around? Thanks in advance


Regards,
Amit Paul
HCL Technologies

 

[Toost]

Can you try clarify what it is you want help with ?


Regards,
Tomas

 

[amitpaul713]

Hi,

I have attached the pasrt which I created using solidworks Swept cut. The problem is I do not have a draft angle, I have two profiles on the both sides. In solidworks I could create a sweep using the profile, path and two guide curves and the result is easy but however in NX I could not find any option of sweep which would remove material. Please help if there is any other way?

Regards,
Amit Paul

 

[cowski]

in NX I could not find any option of sweep which would remove material

You are probably using the "swept" command in NX. If the result is a solid body, subtract it from the target body; if the result is a sheet body, use the "trim body" command to use the sheet to cut away material from the target solid.

www.nxjournaling.com

 

[amitpaul713]

Hi,

Yeah that is the first thing I tried out. Certainly subtract option is not working out, it shows that the body (created using swept)is a different feature and cannot be subtracted (Sorry for not quoting the exact error message) but unfortunately subtract doesnt work.

Regards,
Amit Paul

 

[cowski]

If subtract does not work, then there is something else wrong; the subtract does not need to happen in the same feature in NX. Perhaps if you posted the exact error message, we could help you track down what is happening.

www.nxjournaling.com

 

[Toost]

above you say that you attached the part, "I have attached the pasrt which I created using solidworks Swept cut. The problem"
But the attachment is an image from Solidworks .( i guess it's from SolidWorks)

?
Regards,
Tomas

 

[amitpaul713]

Hi Tomas,

Yes that is a snapshot from solidworks. What I meant is creating such kind of part is easy in solidworks by using just "swept cut" but is there any such tool in NX like that which I am unaware of? Adding material works fine with the different sweep features in NX. However, removing material is the problem here and the subtract operation does not seem to work out(have tried quite a few times).



Regards,
Amit Paul

 

[MFDO]

Use NX’s "Sweep Along Guide" command with Boolean “Subtract” option.

Michael Fernando (CSWE)

http://www.solidCADworks.com

Tool and Die Designer
Siemens NX V10.0 + PDW
SWX 2013 SP3.0 X64
PDMWorks 2013
Logopress3
FastForm Advance
FormatWorks

 

[amitpaul713]

Hi,

I have attached the file in .step format. Could someone please help me out making this in NX without using any angle (draft angle). There is no angle input to use draft option and I only have two profiles on the both opposite faces, so what I did is I created 3D curves by joining the reference points and then used swept cut (in SolidWorks) but I cannot figure out the same in NX.

Regards,
Amit Paul

 

[amitpaul713]

Hi MFDO,

Sweep along guide will only allow one guide curve and that will not allow me to get the shape I want.

Regards,
Amit Paul

 

[cowski]

Here is one option (NX 9 file format).

http://files.engineering.com/getfil...783-496a-8218-54560222f833&file=swept_cut.prt

www.nxjournaling.com

 

[DonNX]

Hi,

What version of NX are you using?

You need to draw the two profiles you want (in your case triangles), one on either end of the block.
Then you need to join the corresponding points with curve lines.
Then using the swept function select the one triangle (section) & the 3 guide curves you created (guides, remember to use "Add new set" for each line).
You should now have a solid body that you can subtract from your block.

If you want I can upload the model in NX8.5.

 

[amitpaul713]

Hi DonNX,

I tried the same way you told at first. But unfortunately subtract doesnt work out for me. It will be great if you could upload the file in NX 8.5.

Regards,
Amit Paul

 

[DonNX]

Here is the model I created:

 

[Toost]

What's wrong with Cowskis model ?
It can't be done much simpler.
In case you for some reason must do it using solids instead of a sheet body and trim, you simply close the triangles, this will produce a solid body instead of a sheet, and then use subtract instead of trim body.

In this case there is no need to complicate things by using a sweep, a Ruled surface or Through curves with two sections will produce the expected shape.
remember to tick the "preserve shape" option to get as simple as possible faces / logical face division.

Regards,
Tomas

 

[amitpaul713]

Hi DonNX,

Thanks! A quick question, what did you use to join the two sketches? I was using spline to join the two sketches and then used swept command by considering the splines as guide curves. Was that the issue that I was not able to subtract?

Regards,
Amit Paul

 

[DonNX]

Hi Amit,

I assume that this method worked for you?

In the one I used a line (Insert> Curve> Line).
In the second I used sketches.
In both cases I used them as guide curves.


"It is impossible to make anything foolproof because fools are so ingenious."

 

[amitpaul713]

Great! That works. Thanks

Regards,
Amit Paul