Line Style change due to Format

[rbreyette-2]

I have a line style question when I print out to PDF.

On the B size format the part prints out with more dashes and dots. (see image)

On the G size format the part prints out with less dashes and dots. (see image)

Does anyone know how I can get the part on a G size sheet to look more like the part on the B size?

The pen tables are the same, and the way I exported the drawing to PDFs are the exact same.

This leads me to believe that the format is driving the way the part looks, sound right?

Thanks in advance for your help.

[MartinHanak]

Ryan,

please upload drawing files.

Martin Hanak

[rbreyette-2]

Martin,

Thanks for responding. Unfortunately I cant due to the restrictions my company has. I was only allowed to do those 2 screen shots. Sorry about that. I know it might be tough to answer without all the info you might need.

But I can tell you the drawing files are the same. They are actually on the same drawing just different pages with dif. formats. They look the exact same in Creo Drawing but change when export to PDF.

Hope this helps any. If not, thanks for trying to help.

-Ryan

[TomD.inPDX]

I thought there was something like a hardware font setting that controls this. However, I would think that the G-size would have a lot more dashes.

Line fonts has always been a mystery to me. One of those black-box-magic things that only PTC gurus manage with a special brew.

[MartinHanak · Accepted solution]

Ryan,

the size of font in PDF is related to size of the drawing. This is default Creo behaviour.

This means ...

>>> small size drawing contains short line segments

>>> large size drawing contains long line segments

To get requested result, you have to modify drawing configuration.

For example, imagine that you want to use PHANTOMFONT and that repeated piece of the font could be 0.2 inches long. In such case you have to add the following option into drawing configuration file:

line_style_length PHANTOMFONT 0.2

See attched files for more details.

Martin Hanak

[TomD.inPDX]

Thanks Martin.

This is worth noting:

line_style_length

line_style_length

sets the font length for two-dimension sketched entities

you must add this option to the detail options file whenever you want to modify the length. you must also set the detail option axis_interior_clipping to no.

the length measurement is controlled by the drawing_units detail file option.

default and available settings

• font_name default*—type the font name and then a desired value for the font length in system units. the "default" setting indicates default length values.
• font_name value—type the font name and then a desired value for the font length in system units.

note

after you add line_style_length to the detail options file, you cannot delete it by deleting the row from the file or by retrieving a different dtl file into the drawing. you must change the value of this option to default to eliminate the option from the detail options file. use the following format:

line_style_length font_name value/default

where font_name is the name of the font that you want to modify, value is the desired value for the font length in system units, and default tells the system to use the default length value.

Here is a nice collection of font names (unverified)

line_style_length CTRLFONT_MID_L 0.400000

line_style_length PHANTOMFONT_S_S 0.400000

line_style_length DASHFONT_S_S 0.400000

line_style_length CTRLFONT_S_S 0.400000

line_style_length CTRLFONT_L_L 0.200000

line_style_length CTRLFONT_S_L 0.300000

line_style_length DASHFONT 0.400000

line_style_length PHANTOMFONT 0.400000

line_style_length DOTFONT 0.400000

line_style_length CTRLFONT 1.000000

[rbreyette-2]

Thanks guys, I will give these a try and let you know how it works.

-Ryan

[rbreyette-2]

Just wanted to update you all. What you both provided worked! One of my guys that knows a little more about line styles was unaware that you could add a value to the end of the line_style_length PHANTOMFONT "0.2". That was a good find.

Doing this trick does casue some other line style stuff to misbehave but I am sure if I work with the other line style info provided by Antonius I can get it to they way we want it.

Thanks for all your help.

[LawrenceS]

Also, how do you get teh line_style to automatically update after changing the value?  It doesn't seem to want to do it unless I create a line and once I change to that line style all lines on that drawing get updated, but not necessarily until then.  I tried Refresh, Update sheets, and even "regenerate".

[LawrenceS]

I see that every time I change between a metric and English detail files that it keeps adding new lines and that as you said I cannot remove a line.  Do you do this using detail files to change the value, mapkeys, or are you manually changing the value?  I cannot see how to get it to work via detail file or mapkey.  Can someone let me know how to do this?

Thanks,

Lawrence 

[LawrenceS]

For completeness, I am going to list the same options that @TomD.inPDX listed, except using the default designator which removes the option from the drawing as he stated.  These can be applied manually, or simply by applying a company detail file with these lines in them.  I tested both on Creo2 M200 but only for "Dashfont_S_S".

line_style_length CTRLFONT_MID_L DEFAULT

line_style_length PHANTOMFONT_S_S DEFAULT

line_style_length DASHFONT_S_S DEFAULT

line_style_length CTRLFONT_S_S DEFAULT

line_style_length CTRLFONT_L_L DEFAULT

line_style_length CTRLFONT_S_L DEFAULT

line_style_length DASHFONT DEFAULT

line_style_length PHANTOMFONT DEFAULT

line_style_length DOTFONT DEFAULT

line_style_length CTRLFONT DEFAULT

[ZRJ]

It's almost as if PTC is trying to lose customers, I'm nowhere near skilled enough to know why it's such a difficult task to get things to print on pdf, the way we we see them on our screen, in the drawing (like any other CAD program)?  As well, why adjusting these line scales is almost impossible, I've found that the above methods do not help if you have large metric assemblies.  It seems these values (even when the model or part file driving the drawing is set to metric) are only inputs of ansi units, and have a max adjustable range or something.  Similar to when you try to do an extrude, and it says must enter a range, some random af range, you want 0.25" but it says sorry must be more than some seemingly random number.

We just updated to version 8.0.10, still no spell check either lol

[Anguraj_K]

Hey @MartinHanak , I cannot find the "line_style_length" option in creo 4.0 and I really want to adjust the setting. Do you where the option is moved to? 

[MartinHanak]

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@Anguraj_K wrote:

Hey @MartinHanak , I cannot find the "line_style_length" option in creo 4.0 and I really want to adjust the setting. Do you where the option is moved to? 

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Hi,

I think you have to type the option manually. See below

[xujh]

Thanks a lot for your help.

I came across one issue in the test. No matter how I changed the values for DASHFONT or DASHFONT_S_S, the hidden lines had never been affected. I guess the hidden lines are a bit different from those line fonts, coz the dashes look a bit longer than the spaces, and the scales of pattern varies according to the length of the hidden edges. Do we have to use pentable to control it? What is the default setup? Thanks again.

[MartinHanak]

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@xujh wrote:

Thanks a lot for your help.

I came across one issue in the test. No matter how I changed the values for DASHFONT or DASHFONT_S_S, the hidden lines had never been affected. I guess the hidden lines are a bit different from those line fonts, coz the dashes look a bit longer than the spaces, and the scales of pattern varies according to the length of the hidden edges. Do we have to use pentable to control it? What is the default setup? Thanks again.

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Hi,

yes, you can use pentable to define "the look" of hidden lines. For example:

pen 3 pattern 0.5, 0.2 cm; thickness 0.025 cm; color 0.0 0.0 0.0; half_tone_color