New to NX 5 and forum...where is simplify body?

[NorthwesternDesign]

Hi all! I just switched over from NX 3 to NX 5. It appears as though the simplify body command is gone. Also, whenever I make changes in the customer defaults (background color for instance), it does not affect anything when I close UG and log back in. Also, I had created my own moldbase and standard parts in NX3. However copying those directories over to the Moldwizard directory under NX 5 does not work. There must be some line of text I need to change, but I cannot find it. Any ideas? Thanks!

 

[hudson888]

It is essentially replaced by the Delete face command. Many users preferred selecting the face that they want to remove rather than the boundary as that is the more intuitive workflow. However if you've a real yen to have back the older selection method in NX-5 you can try adding in an enviornment variable to ugii_env.dat. Youll find it by reading the thread below

http://www.eng-tips.com/viewthread.cfm?qid=199883&page=2

Before you do so don't give up on delete face too quickly there are a great many additional selection methods available using the new function which in most cases make up for what you may have lost with the previous method.

Older files will still carry the simplify body features in the tree rather than the newer delete face in order to faithfully support that legacy data so for a time at least you may still be able to gain back door access to the old method if you insist.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[JohnRBaker]

Note that many items set in Customer Defaults are 'part specific' which means that any changes made will ONLY effect new parts create AFTER those changes were made. Note that those items which are 'session specific' those will have an effect on both new and legacy parts.

To get an idea of which items are 'part' and which are 'session' specific, go to Customer Defaults, select the 'Find Default' option (the binocular icon) and enter the word 'all'. When the list comes up scroll to the right to the last column titled 'Scope'. Select the title and it will sort the listing so that you can now review, as you scroll down, all of the items which are 'part' specific and which are 'session' specific.

As you will discover, virtually all of the items which effects the colors of objects and items inside of a part file will be listed with the 'Part' specific group of items. If you wish to permanently edit those aspects of the file, you will need to open the file of interest and make those changes using the appropriate dialog found on one of the menu items under Preferences.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
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.

 

[NorthwesternDesign]

Thanks hudson and John Baker. I was always used to using both delete face and simplify body in NX3, however if there was a parameterized feature, delete face did not work before. I see that it does now. If the model was unparameterized, sometimes delete face would work and simplify body would not or vice versa. I think the delete face makes more sense though.

John, I can see what you are saying about the binocular icon. However, are you saying that after I change the setting in customer defaults (lets say to turn off the grid in drafting and change the background to black in modeling and drafting), when I open a new session of nx5 and create a new part, it should recognize those changes I made? If so, that is not happening.

 

[JohnRBaker]

When you do a File -> New are you selecting one of the predefined templates or the 'Blank' part option? If you're picking a template, you will need to go in and open the template files and using preferences, make your changes and re-save them. If you select the 'blank' part option, it should work as described.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
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.

 

[PheasantPlucker]

Your moldbase and component files should work.Check your moldwizard_catalog.txt file and be sure it points to your files.Also, you may need to add/change a UG_MOLDWIZ_DIR variable to point to the new location.

 

[NorthwesternDesign]

John, I had never even noticed the "blank" option before. After selecting that, I was able to get it to work, but I had to change the Gateway-Visualization-Background Color Tab within the customization to graduated and change all the values to 0. For some reason, when I set both shaded and wireframe views using the plain option, it reverts back to a gray background. Even if under the Color Settings tab in the same menu has the background set to black. Thank you for your help.

 

[NorthwesternDesign]

Thanks PheasantPlucker for your response. If you or anybody happens to know where these variables are that I can change, that would be greatly appreciated. It looks as though I will have to change the moldwizard_catalog.txt files (I found those), however when I copy my old files over to the new NX 5 directory, and put the NX 5 files in a temp directory (while still keeping the map_template_name.txt in its original place, I get the message "Moldwizard kit not found".

 

[PheasantPlucker]

The UG_MOLDWIZ_DIR is a system variable.This is used if your directory is somewhere other than the default location. Is your moldwizard directory on a network drive? If not,
I would copy and paste the "moldbase" and "standard" directories from your NX3 folder to your NX5,overwriting whatever is there. Where does the "Moldwizard kit not found"
message appear?In NX when you start moldwizard?

 

[NorthwesternDesign]

The error message appears in NX when I start moldwizard. (That is after I copied the directories from NX 3). Moldwizard is stored locally on my hard drive. I will try to copy only the moldbase and standard directories to see if that makes a difference.

 

[PheasantPlucker]

This may seem like a dumb reply, but be sure to restart UG after you make any changes. The error message occurs if the moldwizard directory isn't in the standard location. Be certain that it is located under the "Program Files/UGS/NX 5.0" directory. It seems to me that it isn't.

 

[smallwhitedog]

UG Hunter
I to could not find simplify body, so I called GTAC and Here are the steps to set the environment variables to allow the simplify body command to appear on the Feature Operation menu. I spoke with UG support and this fixed my problem of no simplify body command in the Feature Operation menu.
1. Control panel
2. system
3. advanced tab
4. environment variables
5. new
6. variable name: ug11_dmx_nx502
7. variable value: 1
8. restart Unigraphics
I hope this helps you.

 

[hudson888]

Or just read the thread I linked you to above and edit an extra line into ugii_env.dat so that the variable is set when you launch NX.

Best Regards

Hudson

www.jamb.com.au

Nil Desperandum illegitimi non carborundum

 

[JohnRBaker]

PLEASE learn to use the new stuff!!!

If you continue to use old outdated functions you will not be able to leverage the newest capabilities of the system. For example, if you go back to using the old 'Simplify Body' function, you will NEVER be able to create a Journal file which utilizes that command nor will you ever be able to perform a Redo after Undoing a Simplify Body command, both of which you can do if you learn to use 'Delete Face' instead.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
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.

 

[smallwhitedog]

Wow, I just applied delete face to a blow molded duct where I would typically use simplify body to design the blow mold. I basically need to remove all of inside surfaces rendering the duct to a solid body i.e no ISM. In nx3 and previous versions delete face would fail pretty consistently whereas simplify body worked consistently. I am really surprised that delete face just worked on a complex duct I just tested it on. It is now a parametric command as well and allows you to use tangent face in the selection process. Thank you John for pointing me in this new direction, serious improvement over NX3.

 

[JohnRBaker]

I'm glad you found the new 'Delete Face' more capable for your type of work.

Note that I was always a big fan of 'Simplify Body' myself and was able to solve some very tricky modeling problems with it. I also had 'fun' impressing people who were using other CAD tools which did not always have anything similar, however it was one of those functions which was not as obvious as to how it was intended to be used as it could be since you had to stop and think about what you wanted to KEEP rather than what you wanted to REMOVE, a concept which was not always that easy for some people to pick-up on at first. In fact, I learned that some people had to watch someone else use it first before they really understood what the intended workflow needed to be. However, since we made the improvements which we have to 'Delete Face', I find that it is now much easier for new users to understand how to use the function by just following the dialog steps and applying what they've already learned about using 'Selection Intent' to define the desired faces quickly and easily.

John R. Baker, P.E.
Product 'Evangelist'
Product Design Solutions
Siemens PLM Software Inc.
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.