Creo Drawing Problems

[sfarra]

Hi everyone-

We are making the jump from WF 4.0 to Creo 1.0 with Creo 2.0 coming as soon as IT can correct a small issue with the license server (it's about time, right?). I copied my existing config file, start parts, and drawing templates from WF 4.0 to use as a basis for the config for Creo and noticed some issues that I can't seem to remedy on my own:

1. In WF 4.0, my system colors are set for drawings to be a near black background and the drawing template has white borders with yellow text. When I print, WF somehow "knew" that I really wanted the white borders and yellow text to be black, even if I was printing in color. In Creo, using the same drawing setup the white lines on my drawing template print out white (very hard to see on white paper) and the text prints out yellow (also very hard to see on white paper). Even the lines that make up the geometry of the parts are white. If I print in black and white everything comes out alright but some drawings need to printed in color. Any ideas as to how WF "knew" that certain things should print out in black? Creo is just printing things as the color they display on screen and I really hate working with a white background color when making drawings.

2. Located in the drawing template there is a note which we use for drawings notes. It is several lines long and some lines contain just text (i.e. "1. BREAK SHARP EDGES") and some lines contain text and a reference to a parameter (i.e. "2. FINISH: &FINISH"). When the drawing is either opened or first created, everything in the note appears as it should. When I open the note properties, the return characters seem to be missing and the text is all on one line. If I make no changes, the text remains in several lines but if I make any changes, the text displays now in one single line. I have looked at my drawing template and confirmed that this problem does not occur there. I have also found that if I copy/paste the text from the drawing template into the notes for the drawing, the problem doesn't occur again unless I click on "Editor..." in Note Properties. Then the issue comes back even though the return characters are in the editor window.

I know I got wordy with this so I appreciate the time that everyone is taking to read and understand this post!

 

[looslib]

Creo 1 is obsolete and has been unsupported since October 2012!

1) Look for the pen table file. That determines which 'pen' to use for what colors to use when a drawing is printed/plotted. You may have multiple files for different printer/plotter configurations.

2) Haven't tried that yet in my testing.

You may want to join PTC/User and sign up for their forums exploder. It gets a lot more traffic for these questions.

http://portal.ptcuser.org/

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

Ben Loosli

 

[sfarra]

Ben-

Thanks for your response. As a contract design house, we are at the mercy of our clients in terms of what softwares we use so supported or not, Creo 1.0 here we come!

I had a sneaking suspicion that the pen table was my way of solving the first problem but couldn't locate the default table. It turns out that the way I accomplished it was to forget finding and editing the default table and just override it with the pen_table_file pointed to a location on my computer. I created a file called "table.pnt" and located it in the same folder where my config.pro file is. The contents of that file were copied from this post (

http://communities.ptc.com/thread/42877)

posted at the end of this post in case the link doesn't work. In case you didn't already figure this out, Ben, I'm not writing this for your benefit so much as for anyone else who should happen upon this thread.

I'm going to keep working at the note issue and thank you for the link to a new forum that may contain my answer.

! Pen 1 = white entities (object lines)
! Pen 2 = yellow entities (text, dimensions, cross hatching)
! Pen 3 = gray entities (hidden lines)
! Pen 4 = red entities (Highlight - Primary (Dark Red)Selected (Red)Secondary Selected (Orange) All items plot as solid lines:
! Spline surface grid (does not plot in drawings)
! Pen 5 = green entities (sheetmetal)
! Pen 6 = cyan entities (section)
! Pen 7 = dark gray entities (dimmed e.g. tangent edges)
! Pen 8 = blue entities (spline surface grid) [use for drawing perimeter border in format]

pen 1 thickness .035 cm; color 0.0 0.0 0.0
pen 2 thickness .018 cm; color 0.0 0.0 0.0
pen 3 thickness .018 cm; color 0.0 0.0 0.0
pen 4 thickness .050 cm; color 0.0 0.0 0.0
pen 5 thickness .035 cm; color 0.0 0.0 0.0
pen 6 thickness .018 cm; color 0.0 0.0 0.0
pen 7 thickness .008 cm; color 0.0 0.0 0.0
pen 8 thickness .050 cm; color 0.0 0.0 0.0

 

[sfarra]

As an update to anyone interested, my IT department solved the issue they were having with Creo 2.0 and the note issue seems to be fixed in 2.0. So anyone chasing this issue may find it to be a bug in Creo 1.0.