Sweep Profile Sketches 2

[jeffco]

Hello
I have received an existing NX7.5 part file that contains a sweep with 12 underlying Profile sketched sections. Each profile is a simple rectangle but there are tiny radius in the corner. I need to remove the radius and rebuild the sweep. How to? Thanks for looking

 

[cowski]

Each profile is a simple rectangle but there are tiny radius in the corner.

Does this mean that the sketches are true rectangles, but the resulting sweep has a radius in the corner, or that the sketches are rounded rectangles? Is this a sweep or a freeform swept feature? Is the resulting body a sheet or solid?

There may be other options available depending on the answers to the above questions, but in general: if the sketches are rounded rectangles, edit each sketch to remove the radius and extend the existing geometry to create a corner. Depending on the curve selection rule in effect for the sweep it may update OK or it might require reselecting the profiles.

If the sketches are true rectangles but you end up with a radius in the corners, I'd guess this is the freeform swept command. If this is the case, make sure the 'preserve shape' option is checked.

Alternatively, you may be able to use delete face or replace face directly on the resulting geometry to get what you want.

 

[JohnRBaker]

If the issue actually is that you have a dozen sketchs with small fillets at the corners and you want to remove them and quickly fix-up your sketches, try this:

Using the sketch editor, perform the following steps for each sketch.

Select the sketch and do an edit. When the sketch editor comes up, select the small arcs and delete them. Now select the sketch icon 'Auto Constrain' and when the dialog opens, toggle OFF all of the option except 'Coincident', set the 'Distance Tolerance' to something greater than the radius of the deleted arcs, select all of the curves in the sketch and hit OK. You should now have a complete closed profile.

Repeat this for each sketch and you should be good to go.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.com/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[jeffco]

John. Your explanation seems somewhat easier to follow than Cowski. Thank you both. Thing is that i do not see the sketches in the browser anywhere. When i right click the feature and choose "Edit Parameters" I see Section-1 thru 12 in the list of sections used to build the sweep. Cannot start the "Sketch Editor" Cannot find the sketch or sketch editor.

 

[JohnRBaker]

Just because they look like 'sketched' profiles they may just be loops of dumb curves. In that case they will NOT show-up as sketches in the Part Navigator nor will there be any options to edit them as sketches, since they aren't.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.com/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[cowski]

If they are dumb curves:
[ol]
[li]Right click on the swept feature and choose 'show parents'. All of the geometry used to create the swept will become visible.[/li]
[li]Suppress the swept feature.[/li]
[li]Delete the arcs you don't want/need[/li]
[li]Extend the remaining geometry with the 'trim' or 'trim corner' command (found on the Edit -> Curve menu).[/li]
[li]Edit the swept feature (right click -> edit parameters); ensure that the section loop arrows are all pointed the same direction (all loops clockwise or counter clockwise, either is fine but they all must match) and start on a similar leg of each rectangular section. Edit sections to change direction or start curve until these conditions are met.[/li]
[li]Make sure the 'Preserve shape' option is checked (it is in the 'settings' section of the swept dialog, you may have to expand that section to see it)[/li]
[li]Unsuppress the swept feature[/li][/ol]

 

[jeffco]

Hi Cowski. that was very close to describing my scenario and what needs to be done. Regretfully, i could not delete the arcs that are at the corners. only Hide them. When i extended the resulting lines, the re-built sweep keeps exposing the arcs and the original profile with arcs and clings to it. Rats! that seemed so close. thanks. i'll keep trying

 

[cowski]

In that case, skip step 3 (for now) and in step 5 (after extending the required geometry) select a section then deselect all geometry and reselect only what you want. Again, make sure the loop direction and start curve is similar to the other sections. Repeat for all sections and unsuppress the swept feature. You should now be able to delete the unnecessary arcs.