Any way to assign linetype scale when exporting DXF/DWG format drawings?

[M_C_Anderson]

I have a drawing with multiple dashed line fonts. In Creo Parametric, the spacing of these line fonts changes dynamically as I zoom in and out so that they are always readable. When I publish the file to a DXF or DWG format, Creo appears to be assigning a linetype scale factor that I cannot control. When I import the resultant DWG file to AutoCAD, I can use the LTSCALE command to enter a new scale factor. I see when I do this that Creo has assigned the factor 2.585 for this particular drawing. Other drawings have their own scale factors applied, I assume based on the size of the drawing sheet (larger sheets get larger scale factors, resulting in wider spacing). Is there any way within Creo to pre-assign the scale so that we do not have to post-process it in AutoCAD?

[MartinHanak]

Hi,

you can test detail option line_style_length mentioned in  https://www.ptc.com/en/support/article/CS378566 document.

[M_C_Anderson]

Thank you for the suggestion. Unfortunately, changing those values (I tried 1, 0.5, 0.1, and 0.01) has no visible effect on the DXF/DWG publish.

[MartinHanak]

---

@M_C_Anderson wrote:

Thank you for the suggestion. Unfortunately, changing those values (I tried 1, 0.5, 0.1, and 0.01) has no visible effect on the DXF/DWG publish.

---

Hi,

1.) what option did you enter ?

2.) did you see the change in Creo ?

3.) can you create and upload testing data ?

[M_C_Anderson]

1) I entered the following options in my drawing detail options:

line_style_length PHANTOMFONT_S_S 1
line_style_length CTRLFONT_S_S 1
line_style_length DASHFONT_S_S 1
line_style_length PHANTOMFONT 1
line_style_length DASHFONT 1
line_style_length CTRLFONT 1

Then I changed it to

line_style_length PHANTOMFONT_S_S .01
line_style_length CTRLFONT_S_S .01
line_style_length DASHFONT_S_S .01
line_style_length PHANTOMFONT .01
line_style_length DASHFONT .01
line_style_length CTRLFONT .01

2) I did see the change in Creo Parametric:

Size 1:

Size 0.01:

However, the resultant DWG exports look identical:

Size 1:

Size 0.01:

And for extra verification, here is a set of screenshots from AutoCAD, showing how Creo has chosen the LTSCALE value of 0.9350 for this DWG export.

Size 1:

Size 0.01:

3) Test data is attached in the line_style_length_test.zip file.

[MartinHanak · Accepted solution]

---

@M_C_Anderson wrote:

1) I entered the following options in my drawing detail options:

Then I changed it to

.....

Hi,

I did some research and found no solution.

1.]

According to https://support.ptc.com/help/creo/creo_pma/r9.0/usascii/index.html#page/data_exchange/interface/Mapping_Layers_and_Line_Styles.html document, user can map Creo line styles to AUTOCAD line styles.

Unfortunately Creo provides fixed list of AUTOCAD line styles, only. Although the user can define his own AUTOCAD line style, he cannot use it during DXF export in Creo.

2.]

DXF export in Creo does not enable user to "stroke" non-solid lines into separate segments which are then displayed in AUTOCAD.

[M_C_Anderson]

Thanks, Martin, I appreciate you looking into this. I'll add this as an idea. I'll go ahead and mark your response as the solution, since I don't think it will be possible to do what I'm asking as Creo currently exists.

Edit: idea post here