Creo goes to not responding mode after click on Table menu

[Devidas]

The CAD data is saved on shared drive.

When we open the drawings and click on Table Menu, it shows the spinning logo initially and creo goes in not responding mode for around 20-30 min. I am using the Creo 2 M120. I have tested this issue with M070 and it shows the same behavior. This happens on Dell and HP hardware.

Any idea or suggestion will be helpful.

Thanks in Advance.

[TomD.inPDX]

Create a support case.

[dschenken]

I worked at a place like that where the computer would flake out for 25 minutes on a save. I figured it was a bad network issue with Windchill, but they had no support contract, and didn't care that I was losing that much time. It wasn't even consistent. Most saves were 10 seconds, but every so often, soaking up a few hours each day - nada. I would preemptively disconnect the Windchill link and that worked, but made using Windchill sort of difficult.

Fire up task manager or Process Explorer to see what the computer is busy with when it flakes. If the CPU is idle and no memory is being allocated, it's probably a network problem; this assumes Creo comes back and hasn't simply stalled and stopped. It's possible it is paging itself to death and you need more RAM, or it's waiting for a network connection - lots of possible areas.

[Devidas]

we are not using Windchill in this case, all data get saved to network drive.

I have opened a case with PTC but they says it may be network related issue. I am not completely agree with that as issue is with test system located in same LAN network of share.

Also it goes not responding mode only after click on table menu and not others.

[dschenken]

The only option is to debug the problem. There isn't a delay-table setting.

1) Does this happen on freshly created drawings?

2) Do the drawings have associated models?

3) Are the tables Repeat regions?

4) Does this happen if you do a back-up of the drawing to a local drive and retrieve from the new location?

5) What does Process Monitor show is happening?

6) Were these drawings made with an older version of Creo/ProE and are just now being opened?

7) Was Creo put on the computer as a clean install? People doing manual copying miss parts and this produces weird results

😎 Is Creo installed locally?

9) Is the license manager installed locally?

10) Is this the same on all the computers or is this only tested on one computer?

[Devidas]

1) Does this happen on freshly created drawings?

--> Issue with new and old drawings also.

2) Do the drawings have associated models?

--> Yes

3) Are the tables Repeat regions?

--> All tables from format only no repeat region tables are there.

4) Does this happen if you do a back-up of the drawing to a local drive and retrieve from the new location?

--> Its not happening on local disk but we didn't get a chance to test will all data on local disk. As share drive have almost 16k files in it.

5) What does Process Monitor show is happening?

6) Were these drawings made with an older version of Creo/ProE and are just now being opened?

--> Yes some with Old version and some are already updated with Creo 2 version.

7) Was Creo put on the computer as a clean install? People doing manual copying miss parts and this produces weird results

--> Yes, its clean OOTB install and even I tried to reinstall it but shows the same issue.

😎 Is Creo installed locally?

--> Yes

9) Is the license manager installed locally?

--> license server is different

10) Is this the same on all the computers or is this only tested on one computer?

--> It shows the same behavior on 3 systems out of 7 systems.

Creo goes to not responding mode only after click on Table menu and no other menu or during open the drawing files so not sure is it network related issue or some table menu issue.

[dschenken]

You don't need to move all the files - open a drawing that creates delays and use Backup to locally store that drawing and its related files locally. Then erase in-memory and then open the drawing from the Backup.

So far I'm still leaning to a network problem. Mis-configured network adapters, bad wiring, mis-configured switch.

I would also look to see if all the search paths are identical - format tables get their information from related models; if the software is looking for models that it can't find to fill out tables, it could cause a problem that only some machines would have and that would depend on the machine.

I started to make a list of all the settings that might result in network access. It starts with ones related to drawings and models. After the dash are ones that wouldn't affect what you are doing, but it's an incomplete list because there are probably 100 or more settings.

use_temp_dir_for_inst (Yes/no)

search_path

search_path_file

start_model_dir

pro_dtl_setup_dir

pro_format_dir

pro_note_dir

pro_palette_dir

pro_symbol_dir

pro_table_dir

regen_backup_directory

pro_group_dir

excel_analysis_directory

external_analysis_directory

file_open_default_folder

mfg_start_model_dir

pro_font_dir

pro_library_dir

pro_material_dir

pro_surface_finish_dir

---

default_layer_model

autodrill_udf_dir

campost_dir

gpostpp_dir

mfg_process_print_dir

mfg_process_table_setup_dir

mfg_process_template_dir

mfg_setup_dir

mfg_template_dir

mfg_udf_info_setup_file

nc_autodoc_param_dir

nc_autodoc_report_dir

nc_autodoc_setup_dir

nc_autodoc_template_dir

ncmdl_bar_stock_part_path

ncmdl_billet_stock_part_path

[Devidas · Accepted solution]

In Creo Parametric 1.0, when the ribbon and tabs were introduced, PTC introduced the cascade gallery for Table > Quick Tables. The gallery shows a preview of the tables in the pro_table_dir, along with previews of recently used tables, system table etc., making it easier for the user to choose which table (s)he wants to insert in the drawing.

As out of the box there is no value set for pro_table_dir option in config.pro file, so its look into working directory which having around 16k files in our case. This is the reason Creo goes to not responding mode after click on table menu and takes around 10-30 min time to get it back.

The workaround on this issue is set the empty folder/directory for this option so Creo will not search the Working directory.

[dschenken]

Where was the working directory?

[Devidas]

Working directory is set as Shared folder and which having the 16k Files.

[bd'mello]

Excellent

This fixes the issue. 

Thanks

[RS_8699895]

Hi, 

I had faced same issue. It got solved now.

But I have one more issue. If I need to select the table, it takes too much to time. 

Please suggest any idea to fix this issue.