The pentable issue rears it's ugly head again...

[Patriot_1776]

Couldn't find my other thread so...

I'm in Creo 3, M130

I've found some other threads about it, and copied what text I could, and it all didn't do a d@mn thing.  I read that the filename of the ".pnt" file could be anything.pnt, but is that correct?  It SHOULD be, but.  I have the config.pro settings:

pdf_use_pentable  yes

use_8_plotter_pens yes

pen_table_file C:\FRANK\(C) PROE\(C) CONFIGS\franks_pentable1.pnt

So that should be ok, and my actual file is:

!PEN1 = Geometry (White)

pen 1 thickness .020 in;

!

!PEN2 = Drawing text (Yellow – dim lines and extension lines, leader lines, centerlines, etc.)

pen 2 thickness .015 in; color 0 0 0; letter_color; selected_color; shaded_edge_color

!

!PEN3 = Hidden Line (Gray - hidden lines, dashed lines, phantom lines, etc.)

pen 3 thickness .015 in; color 0 0 0; sketch_color; curve_color; primary_highlight_color

!

!PEN4 = Highlight - Primary (Dark Red), Selected (Red), Secondary Selected (Orange)

pen 4 thickness .015 in; color 0 0 0; geometry_color; edge_highlight_color

!

!PEN5 = Sheet Metal (Dark Green –Sheet metal solid geometry)

pen 5 thickness .020 in; color 0 0 0; drawing_color; preselection_highlight_color

!

!PEN6 = Sketched Curve (Blue - Sketcher section entities)

pen 6 thickness .015 in; color 0 0 0; quilt_color; hidden_line_color

!

!PEN7 = Highlight - Secondary (Dark Gray - Toggled sections, Grayed dimensions/text, Dim tangent edges

pen 7 thickness .015 in; color 0 0 0; datum_color; previewed_geometry_color

!

!PEN8 = Highlight - Edge (Green - Spline surface grid)

pen 8 thickness .015 in; color 0 0 0; dimmed_color; section_color; background_color

Any ideas?

Thanks!

[TomU]

Pen table file name and extension can be anything you want.  You just need to make sure the config option matches.  Our's is:  pen_table_file H:\Library\Plot\pen_table.txt

I'm not sure spaces and parenthesis are allowed in the file path.  Might need to remove those...

pen_table_file C:\FRANK\(C) PROE\(C) CONFIGS\franks_pentable1.pnt

Everything else looks okay...

[Patriot_1776]

'Sup Tom!

I copied straight from the Windows explorer path that shows up when you highlight the bar, and Creo recognizes the path to my syscol.scl and tree.cfg file (same exact folder).

This is kinda p!ss!ng me off.  Never played with a pentable before.  I'm gonna try a REALLY drastic change and see what happens.

[Patriot_1776]

I made a change to .060" to the text dim lines, extension lines (yellow), and got zero change.

There's gotta be something else...

[TomU]

Are you testing this by creating PDFs, printing, or looking at the print preview?

What happens if you name the file table.pnt, drop it in your working directory, and point the config option this this location? (Just to test.  I'm still suspicious of the spaces...)

I've attached a copy of my pen table file.  I'm positive this one functions.  Maybe see if this works in your test location.  Keep in mind that you will probably need to restart Creo to have any changes take affect.

[Patriot_1776]

Interesting file.  You're using .003" for geometry lines?  Is there a scaling factor when printing, because drafting specs put geometry lines at .020", which is what I set mine to, and my text/dims are set to .015"

[TomU]

Funny you should ask.  There has been an ongoing "discussion" here lately about this very thing.  The current values were selected many years ago (circa. WF3 days) based on what people wanted to see on the prints.  About a year ago I switched our fonts out to use the new ASME compliant TrueType fonts.  Compared to the geometry lines, all of the new fonts look way thicker and bold.  The solution is to thicken everything else up (more in line with ASME standards), but this is VERY different from what we've been producing for the last 30 years and not seen as acceptable to most people.  The major concern is the loss of detail between closely spaced lines.  The individual lines are very distinct at .003" but turn into a big blob at .020".  Not totally sure what to do yet...

[Patriot_1776 · Accepted solution]

Well, maybe I have the answer!  Ok, so, after F@#$#$% with it most of the day, what I found was:

1.  The path didn't matter, it worked the same as the syscol.scl, and .dtl files etc.

2.  The FILENAME seemed to matter (like it does for config.pro vs franks_config.pro or syscol.scl vs franks_syscol.scl, so I just used pen_table.pnt

3.  I believe the text and/or formatting in the .pnt file matters because my file was exactly like yours, but it wasn't the same file.  Dunno, but as soon as I simply changed the values in your file for pen weight, and made sure the paths worked, BOOM!, everything worked.  I wasn't gonna spend time trying to debug the "code" of the .pnt file, I was just happy it worked.  So then I tweaked the numbers until I got a nice heavy line for geometry, and a lot thicker one for dimension/extension lines, centerlines etc. than I was getting before playing with the pentable file and what your file gave me.  And got one that was noticeably thinner line than the geometry line, yet a LOT more readable.  We sign then scan the signed dwg PDF's and add them as attachments (along with STEP files and vendor data) to our dwgs, so, you simply couldn't see the dimension or extension lines or centerlines at all after the scan, it totally $ucked.  This is gonna work WAY better, thanks guys for your help, and I've attached the numbers I came up with for line thickness.

@ptc:  You guys REALLY need to change things with the pentable file and how all that works, and make line thickness variable by TYPE of line, not COLOR.  For instance, I use phantom lines for tangent edges (i.e. for rounds) and if I was on the drafting board they would be the same lineweight as centerlines, dimension lines, etc.  Because lineweight is set by COLOR, those lines are white, meaning they print the same thickness as geometry lines, which is incorrect.  OR, better yet, you should change any tangent lines like that to a COLOR that will print thinner.

Anyways, y'all give it a spin and let me know what you think!

[TomU]

I wondered if maybe there was something in the file.  I've had it before where the file just completely stops working.  I think it might have something to do with the editor used and hidden characters (carriage return, line feed, etc.)  Now that you have it working, I bet you could change the name to whatever you want and it will continue working fine (as long as the config option matches.)

[Patriot_1776]

'Morning Tom!  Yeah, there's some voodoo going on in there for sure!  Nah, I'm gonna let THAT sleeping dog lie!  At first I cut&pasted your file into Word, added some comment lines....and it didn't work.  when I simply copied your file and changed the numerical values for width, now it works.  I really like the way things look and print now.  Not perfect (heavy tangent line issues as noted above), but perfect enough.  I'm going to pass this around to users and the admins at work and hopefully it'll be implemented.  I'd like to think all the work I did would help others here instead of just me.   This has been bugging me since I got here, and I really think this should have been done at the Admin level since they're the ones who set other standards.  But, hey, I got to play Admin on TV yesterday, so...

Did you try it?  Thoughts/comments are very welcome!  🙂

[BenLoosli]

NEVER use Word for editing text files for Creo. Use Notepad, Notepad++ or Wordpad. Word has many imbedded characters and formatting commands that you do not see that mess up the data when a program is looking for a simple text file.

I took a simple file created in Notepad and it is 1K in size. Same text data in a Word file and the file is 14K in size. Lots of bloat in a simple file to make it look pretty!

[Patriot_1776]

'Morning Ben!

That makes total sense.  I just didn't like the formatting in notepad (there are no margins), and it wouldn't recognize the .pnt file, I had to copy it as a .txt file, then copy it back, so, I got tired of that and went to Word because it recognized it as-is and I could edit it there.  I'll try wordpad.  For reference, the pen_table.pnt as saved by Word is only 1kb.  Yeah, leave it to Micros3ck to bloat everything with hidden garbage...  😉

[Dale_Rosema]

I would recommend Notepad++ if can use that.

[MartinHanak]

Hi,

1.]

Copy franks_pentable1.pnt into C:\FRANK directory.

2.]

Set pen_table_file C:\FRANK\franks_pentable1.pnt in your config.pro file.

3.]

Start Creo and check whether your config.pro is loaded.

File > Options > Configuration Editor.

4.]

Open drawing.

File > Print > Print > Settings > Printer tab > check the contents of Table file field

[Patriot_1776]

Thanks for the reply guys, I think the license server is down now since I can't even get into Creo.  I'm gonna try Tom's file in C:\TEMP and see if that's it.  Like I said, the colors and tree files work fine, so, I'd be surprised if there was an issue with that same folder just because it was looking for a .pnt file.  But, it IS Creo, so...  😉

[Patriot_1776]

Oh, and is it egotistical and/or self-centered to mark my own solution as "accepted" if it actually IS the solution?  Just trying to get that "diamond" rating, Yo!  LOL  🙂

[Patriot_1776]

Sooo....did anyone give this a spin and see how it printed for them?

[Patriot_1776]

Crickets?

[Dale_Rosema]

Took the moment to check. Nothing notably different from my pen table where everything is set to .02. Had a colleague check to make sure I didn't miss anything. 

[Patriot_1776]

'Sup Dale!  Interesting.  At least for me, there is a clear and marked difference (improvement) in the thickness of the dimension, extension, and centerlines etc., making them a lot more readable, and now there is a very clear difference between object/geometry lines and these thinner ones.  If it's not much different for you, then you had a much better pentable than I got stuck with standard!  🙂

I'm sure we spent a metric $h!te-ton of money when we got Creo, I'm disappointed that the people we hired (dunno who that was) to install Creo didn't take the time to make sure the printing was up to drafting standards.  I think many times that IT people setting up CAD systems don't even know that these systems are to create DRAWINGS, and that there are drawing standards that need to be followed for readability.