Promotion of Bodies procedure icon

[walkersea]

I have read through the "promote" threads and have a weldment that ideally suits promotion and then finish machining.

In the help section, it states:

Promotion of Bodies Procedure

1. Open an assembly. The assembly must be the work part and the component containing the body you want to promote must be loaded.
2. Choose the Promotion of Bodies icon.
3. Select the desired body.
4. Choose OK.

I can't achieve step 2 as the icon is not visible. I can't find it in any of the menu add or remove buttons or the pull-down menus using NX3 (version 0.0.21)

The help mentions a switch:

You can convert a promotion to a linked body by setting the environment variable UGII_CONVERT_PROMOTION_TO_LINKED_BODY is to 1.

What does this mean? Does this have to be set to allow the promotion of bodies or is it a special case "promotion to a linked body"?

Is there a menu-mapper anywhere - i.e. the location of the reference command icon in the standard toolbars or on the pull down menus?

Help greatly needed!

 

[Shadowspawn]

Walkersea,
Promotion of bodies 'can be' thought of as a legacy holdover from earlier versions of UG. I think the favored route is to 'wave-link' the geometry instead of promoting the bodies. The basic idea is that you want to make an 'associative copy' to work on.
This being said, in NX3, you can access the icon by; a) <Insert> <Associative Copy> <(pick one...) Wave geom linker -or- promote body>, or b) from the assemblies tool bar, pick the wave geom linker (it looks like two links of a chain.
I'm assumming you know how to modify your settings to show icons (tools, customize, ... ). You can fully customize the user interface here by turning on various icons, etc.
Clear as mud? Hope this helps...


Regards,
SS
CAD should pay for itself, shouldn't it?

 

[Xwheelguy]

walkersea,

First of all, I believe there are some Customer Defaults that you need to set in order to allow interpart modeling. Open your customer defaults and from the list on the left side of the Customer Defaults dialog, select Assemblies then General. Make sure 'Allow Interpart Modeling' and 'Allow Feature Promotions' are both checked. Click Apply then OK. You may have to acknowledge that your Customer Defaults are being changed. If so, click Yes or OK.

Finally, exit out of NX and restart NX. See if the icon in question is now available. If it's not, make absolutely sure you have everything set up as you defined in the 4 steps you posted. Should this not fix the problem, post back and we'll take a closer look.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

 

[walkersea]

Thanks guys, but unfortunately neither gets me my icon!

I have checked the customer defaults file and both options are ticked. I have also noticed that using the Insert.. Associative Copy.. only gives me the WAVE Geometry Linker.. option, nothing else.

The only reason I wanted to use promote is that the particular application matches the recommended route in the help system. If there is a way of getting to the same point with WAVE that's OK, but I only have the solid models, assemblies, etc not the full WAVE functionality.

How could the following be achieved?

2 off plates 200mm x 100mm x 12mm thick, welded to a cross member of 80mm AF SHS 6mm thick to effectively make a U shape lifting piece. Post welding, a through bore is added to the lugs of the U (otherwise distortion during welding means the tight fitting pin doesn't pass through the holes).

The problem is getting NX3 to let me do this - will WAVE ing do it and if so what are the steps required? I had a quick go but the linked body is only allowing the hole through one plate, not right across the assembly - the WAVE function has just copied the three parts, not "stitched" them together to be a effectively a single part. I do not want to unit the bodies as then I lose the weld joint lines.

 

[ewh]

It won't recognize a single body unless they are united as a single body. If you don't want to unite them, just insert the hole thru both plates individually.

 

[Xwheelguy]

First, just to be sure there aren't any issues in the current version you're using, I'd recommend installing some Maintenance Releases and/or Maintenance Packs if possible. You're using something like the initial release of NX3 and that's usually not a good idea if other versions with bug fixes are available AND your company allows for the upgrade.

The Promotion icon is on the Feature Operation toolbar, at the end. It should be visible no matter whether you have an assembly as the work part or not.

If you can't get this to work, there's a new feature called Assembly cut that would add the hole you're needing without the need for any Promotions. Just get as far as you want with the assembly and make the assembly the work part, then create a sketch for the bore so it's where you want it (I am assuming this is a plain old circle). Extrude the circle so that it passes through both side blocks and create the cylinder. Now click the Assembly cut icon, pick the 2 side blocks as targets, click the cylinder as the tool and there's your hole. You can turn the tool blank option on (to hide the cylinder) if you wish. Now add the pin using mating conditions or create a new assembly, add the U shape lifting piece and then mate the pin.

This works fine, I tested it out with a simple assembly.



Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

 

[Xwheelguy]

Just a quick follow up regarding Promotions....

I feel there is some sort of misunderstanding about how to use a Promotion in NX, so I'll give you an example that should be easy and work.

We'll build a very simple partial mold assembly that consists of an upper mold, minus the casting. When finished, we will have an upper mold blank, an upper mold "assembly" with the cavity subtracted, and a casting. Editing any component will result in the partial assembly updating automatically.

1. In a new part file, create a block, any size with the bottom face exactly on the XY plane. Save the part as upper.prt.

2. Create a new part called casting.prt. Make a sphere with a diameter that is smaller than either X or Y distance of the block so the sphere doesn't overlap the blocks of the mold. Save the part.

4. Create a new part called upper_assy.prt. Add both parts we created, position them so that the center of the sphere is on the lower-most face of the block and in the center of the lower-most face. We're going to remove a hemisphere from the upper mold.

5. Promote both bodies, then subtract the sphere from the block. Save the part.

6. Switch so that the sphere (casting.prt) is the work part. Change the diameter of the sphere enough that you will notice it visually. Now look at your upper mold. It changed too. If you modify the upper mold component, it will update as well.

This is pretty much how promotions work. All a promotion does is allow you to create features or feature operations that you can't do in an assembly context.

However, you can accomplish this very same thing by using Assembly Cut and I feel it's a bit easier to understand/follow along than promoting. It definitely saves a couple of mouse clicks compared to using Promote.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

 

[walkersea]

Thanks, folks.

I tried the assembly cut route - that is ok for plain holes, but I can't add a thread to the hole (for example), so it is of limited use. Also, some strange things seem to happen with the blanking of the tool body - I have to repeatedly go into the model tree to uncheck the show tickbox - probably something to do with our setup - otherwise the tool body is always shown on the assembly drawing, regardless of its state in the assembly model.

Uniting the parts isn't an option as I need to retain the individual part lines for the weldment drawing.

I could of course add the holes to each plate - but that is just such an inelegant solution! The design intent is for a single through bored hole after the welding operation is complete.

I now have the promote icon (thanks Tim), and have promoted the items as per the help file. However, still can't get the through hole to cut through both plates. I have noticed though that the example in the help file states making two holes, so obviously the functionality just isn't in there. I assumed I'd be able to get the parts requiring the hole to be at the assembly level and use the hole tool on them, but NX still treats them as seperate entities.

I'll try a few more things and add a post if anything interesting turns up.

 

[Shadowspawn]

Walkersea,
A couple of things... 1) Promotions and wave-linked geometry (notice I said geometry and not solids) can be thought of as the same, EXCEPT that wave-linking can involve curves, datms, solids, sketches, blah, blah, blah and promotions deal only with solids. 2) When wave-linking as described by Tim, bring the original component onto a layer different than the layer you want the 'workable' solid on. After linking the geom, turn the original layer off or replace the ref set of the component to empty.
There are ways of getting want you want as far as your holes go. Add a hole through part 1, and note the expression number for the diameter. Place a second hole through part two, and set the diameter equal to the diameter of hole one (diameter hole 1 = p5; dia hole 2 = dia hole 1 -or- dia hole 2 = p5) and anchor the hole to the arc center of hole 1. Your right though... until you unite the two solids, NX will treat them as separate entities so you will have to use two holes and two threads; but that doesn't mean you can't tie the two together so that if position or size changes the one will follow the other (effectively having only one hole and preserving your design intent).
To remove the tool body from the assembly drawing, remove the tool body solid from the reference set being used. I think NX automatically adds all solids to the ref set... or if your using 'entire part' as the ref set, make one with only what you want.
Clear as mud?

Regards,
SS
CAD should pay for itself, shouldn't it?

 

[ewh]

As in most things UG, there may be many ways to accomplish the same thing. The advice given by Tim and Shadowspawn is excellent.

You could also create a sketch of your hole, extrude it twice and subtract each from your parts.

You could create a cylinder, move it to it's own layer, extract two bodies from it and subtract them.

You will come across situations where any of several methods is suffucient, and other times where only one will get you what you need, or at least can use.

Good luck!

 

[Xwheelguy]

Walkersea,

You really don't HAVE to blank the tool body for the hole. To keep the tool body hidden in your drawing, open your Assembly toolbar, hit the Explosion/Create Explosion icon and hide that component that keeps showing up. That will keep it from showing up in your views. Yes, you have to do it in every view UNLESS you hide it in the very first parent view, then all child views will have it hidden as well.

Also, the reason you can't add a thread to the hole is because you have to Promote a body in order to create additional features or feature operations at the assembly level. NX will not allow you to do this without Promotions.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com