fill in holes on surface to machine

[pamccrac]

is there a way to fill in a hole in a surface to eliminate tool from "diving" when machining said surface.

Patrick McCracken
CNC Programmer

 

[Xwheelguy]

You should be able to edit the surface and either use Remove Hole, if in fact it's a true circular hole, or you could try using Untrim.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

 

[pamccrac]

Forgive me, I'm not a "UG" guy. will this work with an IGES??

Patrick McCracken
CNC Programmer

 

[JohnRBaker]

I'm not a 'CAM' guy, but I think that most of the machining routines provide a means to 'skip' over holes and such.

John R. Baker, P.E.
Product "Evangelist"
NX Product Line
UGS Corp
Cypress, CA

http://www.ugs.com

 

[cowski]

For a more roundabout way you could also try to thicken sheet (pick a convenient value - one that works and that you can see) then go to edit face -> delete face (pick the 'hole' surface(s) perpendicular to your surface) and use the 'trim existing surfaces' option. You can now use this surface of the new solid or extract the face if what you need is a sheet body. I have not tried this on an IGES file but I have done similar to parasolids.

 

[Xwheelguy]

Patrick,

Untrim will work on any surface that is in an NX session and not already Untrimmed or at its original size when it was first created (regardless of it being imported or native to NX). Surfaces that are trimmed typically retain the information to allow them to be untrimmed, even when imported from a neutral file format, such as IGES.

For example, let's say you have 2 surfaces that are perpendicular to each other and they have been trimmed back from their intersection by 3rd surface that is a fillet/blend/round of some sort. If you were to use Untrim on either of the 2 surfaces that are perpendicular to each other, they should untrim back to the size and shape they had prior to the fillet/blend/round was applied. I hope that's not too confusing.

This only works on surfaces. If you have a solid, you'll have to extract the face (which creates a surface) and then use untrim.

I'm sure there are several routes you could choose from, but based on the replies here, I'd try looking into the CAM side to see if you can skip over the hole somehow. If that ends up being a dead end, then you might wish to try Untrim or Remove Hole. Untrim will remove any holes and restore the entire surface back to its original state when it was created (regardless of where the surface came from, e.g. imported or native). Remove Hole only removes the selected holes from a surface and maintains the outermost edges as they are.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

 

[pamccrac]

ARE YOU REFERING TO "WHEN GOUGING" - NONE,WARNING,SKIP,OR RETRACT....??

SKIP, in this case, does not keep tool from "diving" at hole location.

Patrick McCracken
CNC Programmer

 

[pamccrac]

tim,

where would i find those commands. I've looked and searched in Help and CAST doesn't find it either

Patrick McCracken
CNC Programmer

 

[TechnicalConsultant]

If you want to remove a hole within NX wouldn't ou be best to use "simplify". This allows ou to pick face/edges etc and remove them.

 

[TechnicalConsultant]

Looks like my "Y" button is getting a little tired : )

 

[Xwheelguy]

noyce,

There's usually more than one way to skin a cat in NX. If you feel simplify works, then by all means use that. However, I choose not to use that and feel more comfortable using Edit Surface (Untrim/Remove Hole). You can still choose edges of holes for removal, but more importantly you can also untrim a sheet back to its original shape if it has been trimmed. Not sure what differences, if any, there might be between using Simplify vs. Edit Surface.

Patrick,

First, you have to be in the Modeling application. Second,
you've never specified which version of NX you're using, so my steps might not be exactly correct if you're using a version other than NX3.

From the NX3 pulldown, pick Edit -> Surface -> Boundary. Select either Edit Original Sheet or Edit a Copy. Next, pick the surface, then choose either Remove Hole or Remove Trim. I'd try Remove Hole first, then pick the edge of the hole you wish to remove. If that doesn't work, use Remove Trim (which to me is Untrim), then trim the sheet back to the original boundaries, minus the hole boundary by using Insert -> Trim -> Trimmed Sheet.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

 

[ewh]

I am not a CAM user, but instead of deleting face, I would use extract face omitting holes, thicken and unite. This way will preserve the parameters.

 

[pamccrac]

nkwheelguy,

thanks for the detailed instructions. I'm using NX1.0.3.2.... I am, however, able to find the boundary command!! The Remove Hole is not allowed, and the Remove Trim works, but a little more than i would like.

I'm not sure I understand about the Insert->Trim->Trimmed Sheet instructions. I've found the command but no luck using it...

did i mention, "working with 'dumb' solids is never fun!"?

Patrick McCracken
CNC Programmer

 

[pamccrac]

ewh,

my question answered!!

thanks!!



and thanks to all for your support!!

Patrick McCracken
CNC Programmer

 

[Xwheelguy]

Patrick,

Once the surface is untrimmed, you will need to trim it back to its orginal boundary, so pick the edges of the other bounding surfaces to trim the untrimmed sheet back to what it was before you untrimmed it, except for the hole.

It's trimming a surface...cutting it down to the desired shape, which is pretty basic modeling. Use other surfaces for the boundaries/trimming objects. For example, if you have 2 perpendicular surfaces that share a common edge (make a corner) and you apply a blend/fillet surface to round off the corner, the 2 perp. surfaces will be trimmed back to the blend's edges. The blend edges were used as trimming boundaries to trim the perp. surfaces back and expose the blend surface. Otherwise, they'd overlap.

For more help, see the documentation for Trimmed Sheet.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

 

[pamccrac]

thanks Tim,

I tried trimming it back, but kept getting an error...

something to the effect, "failure due to gap at edges"

this may be due to the IGES I'm working with. None the less, Extract/Face worked.

I got the tool to quit "diving", now just need it to acknowledge the check surfaces. Working with 5 axis Variable countour method.

Patrick McCracken
CNC Programmer

 

[Xwheelguy]

Yeah...that's the bad thing about having to work with imported geometry...that sometimes ruins the tolerances/gap conditions. I constantly have to untrim surfaces due to those wonderful styling people that run Alias not taking machining stock into consideration, so our surfaces are usually too short and we have to untrim them to get them to meet our casting profiles/surfaces.

Regardless, I'm glad you got it worked out. Just goes to show you there are many ways to accomplish the same thing in NX.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com