Why is pdf export still crap?

[ptc-2053410]

Venting time, why is PDF export still so terrible? Even using a pentable (the work around for the last few years since it has been broken) with the pens sizes turned down to pretty much zero the drawings are aweful. Is it too much to expect for this to work?

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[MartinHanak]

Paul,

can you upload some example ?

Martin Hanak

[BrentDrysdale]

Hi Paul,

Sorry but wrong time zone to reply fully. Took a bunch of work to get this right in WF5 but did get a very good result and seems to still work OK in Creo 2.0

Have to turn off all pen weights and use the table with suitable values and colours (i.e. black). There are plenty of little hooks to trip you up though. I used weights at the lighter end of the scale for A2 and smaller drawings and I cheated for tangent lines as very fine so that they did not overwhelm the parts. This later is especially important if you use dimmed tangent lines in parts and you have several or many internal lines.

Regards, Brent

[ptc-2053410]

The attached image shows pentable settings, location, config options and a comparision of what is being seen when exporting a pdf and what is on screen. All pointing to the right place with all pens turned down to 0.001cm!

The PEN Table may not be working as all the pen thicknesses have been set to be the same thickness, the weird thing is that this has worked previously. I wonder if there is some other setting overiding the pentable? I have had that previously when we changed to creo 2 and we had some setting conflicts from our standard settings causing unusual behaviour. .

[TomD.inPDX]

What method are you using to create the PDF?

[TomD.inPDX]

Remove those entries from the config.pro and make a file named

table.pnt

Add the following to the file: make sure the file does not have a hidden .txt extension

pen 1 thickness .002 in

pen 2 thickness .002 in

pen 3 thickness .002 in

pen 4 thickness .002 in

pen 5 thickness .002 in

pen 6 thickness .002 in

pen 7 thickness .002 in

pen 8 thickness .002 in

Place the file in your working directory (folder).

Use the export to PDF dialog and check the Use Pen Table option in the option dialog.

Now export the PDF.

This worked for me on this file using 600-PDI setting:

That is a 1/8" ball at 1:1 on an A-size drawing zoomed 800% in Adobe reader.

EDIT: I only suggest you try this method 1st to make sure you can get the output you want. After that, follow the steps of the other replies to integrate the settings into your default configuration.

[MartinHanak]

Paul,

it looks like Creo 2.0 does not load your config.pro file ... Can you check if it does read it ? Use File > Options ...

Also check if your config.pro contains the following option

use_8_plotter_pens yes

And the last note ... please tell as what maintenance release of Creo Parametric 2.0 do you use.

Martin Hanak

[rzukowski]

I had a lot of trouble getting PDF's to plot correctly, too. Here is what I ended up doing:

Put the following lines in your config.pro file:

pdf_use_pentable yes

use_8_plotter_pens yes

pen_table_file T:\Engineer\Library_Proe\6_Creo2_System_Files\config\Plot\pen_table_pdf.pnt

"T:\Engineer\Library_Proe\6_Creo2_System_Files\config\Plot" is my path to the "pen_table_pdf.pnt" file.

The pen_table_pdf.pnt is just a text file that contains the following lines:

pen 1 thickness 0.005 cm

pen 2 thickness 0.005 cm

pen 3 thickness 0.005 cm

pen 4 thickness 0.005 cm

pen 5 thickness 0.005 cm

pen 6 thickness 0.005 cm

pen 7 thickness 0.005 cm

pen 8 thickness 0.005 cm

For plotting to the plotter or printer, we use the default MS_PRINT_MGR. The ms_print_mgr.pcf file has a line that calls for the pen_table_ms_print_mgr.pnt pen table file. Make sure to use the correct paths to your file locations.

Hope this helps,

Rick Z.

Attachments:

• pen_table_pdf.pnt.zip (200 bytes)
• pen_table_ms_print_mgr.pnt.zip (225 bytes)
• ms_print_mgr.pcf.zip (285 bytes)