assembly holes 2

[enghoo]

In real life and most (if not all) other cad systems, you can stick parts together in an assembly (eg. a weldment) and then drill ONE hole, ONCE, through all of them. Why can't we do this in NX? Having to promote or wave link the parts, then put separate holes in each of them, then type in the right expression if we want the hole sizes linked, and only being able to dimension each hole off of its own solid is ridiculous. Holes get match drilled all the time, so we ought to be able do the same thing in the cad system without it being such a nightmare. We have over a thousand seats, and I hear this same gripe all the time. The assembly cut feature is at least a start in the right direction, but we finally got a good hole wizzard - we should be able to use it on assemblies. How about if there were something like a macro that runs the hole wizzard then makes a solid that "assembly cuts" through all the parts? Anybody have any ideas?

 

[cowski]

Which version of NX?

If you are on NX6 or higher, look up 'assembly cut' in the help files.

 

[jerry1423]

There is a way to do what you want now. I am not sure if "assembly holes" is in NX7 or what version. I don't have a need for it so I don't use it.
Maybe wait until John Baker gives his two cents worth . . . there is a good answer for what you want.

 

[jerry1423]

Insert > combine bodies > assembly cut

I am in NX6

 

[enghoo]

Sorry, I forgot - NX6.

Thanks.

 

[enghoo]

Thanks for the replies. Here's the problem. Let's say I have a large plate and want to weld a small pad on either side,then drill a normal fit counterbored clearance hole for a #10 socket head cap screw through all three parts, using assembly cut. I have to go look up the hole drill size, the counterbore diameter, and the counterbore depth. Then I have to make a solid to use as a tool, which means either making a new part or building it inside the assembly. If I want to do this by starting with a sketch, I still have to link whatever face I want it attached to, along with whatever edges I want to locate it from, because I can't even make a datum plane associative to a component part. How about if we added geometry to the screws in our library, so you could insert and constrain the screw, then assembly cut the hole with geometry in the screw part? Maybe we could add a deformable part, called something like "sochead_screw_hole" to the library. Is it possible to import the table NX uses with its hole wizard, so to get the right hole you would still only have to know the screw size?

The best solution would still be to fix the software so you can make a hole using "hole", just like in a piece part. Maybe I can run it up the flagpole here and we can get it considered as an enhancement request.

 

[looslib]

Wildfire does it the same way NX does, you have to create a sketch of the shape you want at the assembly level.
Not on NX6, so hopefully Siemens has fixed the Pro/E problem of modifying the details with the cut hole. The cut is only at the assembly and should not modify the original parts.
I know promotion of bodies has been replaced by newer tools, but you could do assembly cuts in V13, if I remember right.

"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[JohnRBaker]

Why not just go to...

Insert -> Design Feature -> Hole...

...and create a Hole using Type 'Hole Series'.

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.org/museum/

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

 

[ewh]

There must be more to it... I try that but am unable to pick any planar surfaces from the components. It seems like it did use to work, but I haven't had the need to use it in quite some time and don't remember all of the right button pushes.

"Good to know you got shoes to wear when you find the floor." - [small]Robert Hunter[/small]

 

[enghoo]

Hi All.

'Hole Series' is handy if you want holes in the piece parts, but that's the problem here; when you're drilling at assembly, you don't want to see the holes in the individual parts. I tried suppressing it at the part level, but then it doesn't show up in the assembly.

There is, however, a relatively happy ending to this saga; I think I've found the least painful way of doing it. You can promote only the first part the hole goes through, and put in the hole just like normal, except down toward the bottom of the dialogue, in the "boolean" box, pick "none" instead of "subtract." Instead of making a hole, it makes a solid you can use as a tool to make your hole. Then do 'assembly cut', pick all the parts you want to drill through, and pick the "un-hole" as the tool. Bingo, you now have a hole wizard hole, through however many parts you like.

 

[hudson888]

Hole series works at the assembly level, and applies similarly to the new hole feature introduced at NX-5. It creates a feature in your assembly, so that each of the drilled through parts carries a link to the hole being added at the higher level.

There's been discussion of the non boolean option before here as well. I guess it works as well as any method. Another way to deal with those kinds of problems that many people use is to simply state drill on assembly on the drawing. I also understand why some people don't follow that process, but it is there as an option.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[JohnRBaker]

If you only want a modeling operation to appear AT the Assembly level and NOT in the detailed parts, then use the Assembly Cut function, as was suggested by cowski in the FIRST reply in this thread.

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.org/museum/

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