Merge two diffrerent files

[par1]

I have only Solid Modeling & drafting module available with UG NX. I wanted to merge two diferent files to check the interference.
(The reason to use merge as we can use that command in Catia V4.)

Could you just explaine me how could i merge two different files?

Thank you,

 

[cowski]

If your end goal is to check for interference, I would recommend starting a new file and pull both your parts in as components (make a 2 part assembly) and run your interference check from there.

If your end goal is to actually merge the files (and I'm unsure what 'merge' means in context of Catia - but in UG I would interpret that as having 2 parts modeled in 1 file), you can export 1 file into the other (File -> Export -> Part... I really DON'T recommend merging the 2 files, even if you think you want to, there is a 99% chance that you really don't. If you try merging them I recommend that you save a copy of each before you do it, so it is easy to undo later.

 

[ewh]

I agree with cowski. If you don't have an assy license, it would be best to import. Open one file, rename it (so as not to lose the original if something goes wrong), make all layers selectable, blank everything. Import the other file, move all entities to an empty layer(s). Now you can unblank all and still have some control between the parts.

 

[cowski]

Oh, no assembly license I missed that when I first posted.

How about if you export a parasolid of part 1 and import that into part 2 (and vice-versa) to check for interference? That way the part will come in as 1 feature (unparameterized feature) and you can easily delete it out of your file when you are done.

 

[par1]

Thank you Cowski & EWH

I applied your 1st reply & it worked without having an assembly licence,
Actually, I am working on battery & one of the hose is passing from the middle of the battery, I am trying to redesign the battery by considering the hose passing through middle of the battery box.(eventually, we need to minimize the battery box to have clerance between battery & hose as per customer requirement)

I tried to subtract the hose to find out how much space i have left to play around but it says unparametric feature?
Could you just explain me how could i find out the
1. remaining space/volume
2. might be the coordinate where it intersects
3. Also how you will sove this problem in UG?

(FYI, I am novice UG user)

Thank you very much in advance,

 

[cowski]

Sounds like the subtract would split the box into 2 or more features (something UG will do IF you are willing to turn your part into a dumb solid - not recommended). As always you have multiple options here. The first thing I would try would be to make the hose into a solid tube (0 inside diameter) and subtract that from the box. You could also just make clearance holes in the wall(s) of the box that the tube needs to pass through.

 

[par1]

I will try that one, I have also one more question with drafting associated with it,

Consider the TOP view, as UG has its own understanding means it takes the view by default.
In my case, all the components are far away from Origin as it was according to the vehicle co-ordinate position.
Now, I wanted to have a view as per my requirement like i created the plane near by that plane & wanted to have a view by selecting that plane.

Eventually, I wanted to select X & Y direction by myself to get the views not as per default. how could I do that?

 

[ewh]

While in modeling, orient your view as you would like it to appear on the drawing. Go to View -> Operation -> Save As. Enter a new view name. You can now place that view on the drawing.