Holes on irregular suface

[ewh]

I have a method of placing holes on irregular surfaces that seems to work well for me. It has come to my attention that "best practices" dictate that there should be only one primitive, if any, in a model. How do others deal with this situation?

 

[ewh]

P.S.
I am not referring to a small number of holes, which are relatively simple to define, but lofted parts with a hundred or more holes.

 

[feadude]

if you use more than one primitive then they are not associated to each other. If you change one primitive parameters then the other primitives are not going to move with this change and they should be moved manually. But you are using holes. Holes are form features not primitives. may be if you explain in more details we will undestand what the problem is. Are these hole positions not fully specified?

 

[ewh]

To use the hole feature, you need a datum plane perpendicular to the surface normal at a point.
When you have hundreds of holes to model (all at differing orientations) this becomes quite labor intensive.
I start with points on the surface defining the hole locations. I offset the surface, create a line using measure distance between the point and the offset surface, then extend the length of the line to ensure it is thru the part. Then it is a simple matter to create a tube (with 0 i.d.) using the line. I then create an extracted body of the tube and subtract it.
To edit the location or orientation, I manipulating the line. To edit the size, I use expressions.
I would much prefer to use the hole feature for this, but find it takes more time and effort to do so.
I am always interested in hearing of more efficient methods to accomplish this.

 

[feadude]

is the line associative?

 

[wmalan]

I'm an NC programmer so I don't follow "best practices" very often. The idea of only one (or no) primitive in a part file is very foriegn to me! I think one would spend a very long time trying to achieve this goal. One would wonder if it is cost effective in complex lofted surfaces. I do see lots of files from aerospace the biggies.

The answer (from what I've seen) is a cop-out. In complex lofted designs, most of the big aerospace firms just leave the holes out. They then use a tab block or just points with info in the notes. I've seen this even with Boeings' Model Based Definition Standard files though they do include the notes within the part attributes. Very common for defining pilot rivit holes. It also allows them to do the ol' change the dimention without changing the model in a "legal" manner.

--
Bill

 

[ewh]

feadude,
The line is the result of analyze->distance, and is not associative.

wmalan,
We just use points for our rivet holes also. They are generally drilled at assembly. The holes I do put in are attachment holes for screws and other fasteners.

 

[J-C]

Are these holes placed at irregular intervals or equally spaced around the perimeter of your part?

Jason

UG NX2.02.2 on Win2000 SP3
SolidWorks 2005 SP5.0 on WinXP SP2
SolidWorks 2006 SP1.0 on WinXP SP2

 

[feadude]

In my opinion and I think UGS as well to be parametric and associative holes should be attached to edges of solid or if this is not possible they should be attached to datum planes that are attached to edges or faces of solid model. Position of holes should be fully specified. This is a practice for the long run and best accuracy. Most of the time extra work upfront will pay off later on down the road.

 

[ewh]

Jason,
Both.

 

[ewh]

feadude,
That sounds great for a big company with deep pockets and far out deadlines, but our situation is different. I can't take a week or more to fully constrain each of these models. The changes that I may have to make later will still be quicker than the initial time investment to constrain them. Most of my time is already taken up massaging and tweaking the surfaces we are given in order to produce parts that meet customer requirements.

 

[J-C]

May not be an option, but since you have solidworks, maybe you could open it in Solidworks and create the holes using a curve driven pattern. Not sure it will hold the holes normal to the surface but I think there are some options there that may.

Jason

UG NX2.02.2 on Win2000 SP3
SolidWorks 2005 SP5.0 on WinXP SP2
SolidWorks 2006 SP1.0 on WinXP SP2

 

[ewh]

Jason,
I like that idea, except I would lose too many parameters (which is the crux of my problem).

 

[J-C]

Well I figure you keep the parameters in UG for whatever associativity and expressions you need to maintain, and then just run the hole pattern in Solidworks as the last feature. I think there's an option in Solidworks when importing a file to maintain face IDs so that updates to the UG file won't cause lost associativity in Solidworks. You have to update the imported body manually though by editing it and reselecting the UG file.

Jason

UG NX2.02.2 on Win2000 SP3
SolidWorks 2005 SP5.0 on WinXP SP2
SolidWorks 2006 SP1.0 on WinXP SP2

 

[HellBent]

You're right on ewh....a good example of the "canned" solid functions taking more time to get the job done.

You said:
"Then it is a simple matter to create a tube (with 0 i.d.) using the line. I then create an extracted body of the tube and subtract it."

I'm not understanding the need for the extracted body?

Here's how I would do it. Create a circle and tube with the "top" of it at zero. Export it to a new part. Then using import part with the wcs set to "specify" you can orient your wcs at the top and perp to each individual line and just keep importing the tube. After you orient your wcs you just select the end point of each line...the tube is imported...then hit "back" to specify the next wcs and so on.

Now as far as editing later on....say the hole size needs to change....editing all those curves could be fairly time consuming. I would probably do it with a surface offset and just do them all at once. I'm concerned with time...which is often not a concern of "best practices".

If there was a command to orient the wcs normal to a surface at a point you could eliminate the need for the initial surface offset and line creation too...maybe a grip?

Take care....

 

[HellBent]

By the way ewh...you wouldn't necessarily have to do the offset and distance analysis. If you have the points you can draw a curve normal to the surface by first selecting the point, then selecting "select face" from the point method pulldown...select your face....then select an end point out in space. You could then do a surface offset and trim them all to the same length with it. Just some thoughts....