I am trying to Export to DWG - Scaling Issues?

[jkmett]

When Exporting to DWG:

1) If the export is a drawing of an "Assembly" the scaling is fine ( geometry,dim, etc...)

2) The Problem:  If the export is a drawing of a "Part" within the assembly something happens:

The dimensions export to the correct value, but the geometry seems to be randomly scaled to some whole number multiple value of the actual part geometry.  I currently deal with this issue by scaling everything by the inverse of that value, and then scale dimensions by the value.

Is there a way to avoid these extra steps?

Thanks.

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[MartinHanak]

Hi,

can you upload some example data (including DWG) ?

MH

[jkmett]

Hello Martin,

The "Wheel Assembly" files attached are an example of correct scaling during the export.  The "Shaft" ( a part in the assembly)  is not scaling properly during the export.

Thanks for your help.@@

[MartinHanak]

Hi,

I tested your DWG files in Draftsight software.

• wheel_assembly_2.dwg ... I created duplicate dimension with same value
• shaft_2.dwg ... I created duplicate dimension to 14.0 with value 42.0

I cannot work with Creo drawings, because they depend on model files ... and ... you did not uploaded them .

MH

[jkmett]

Martin,

That thought crossed my mind, but when I saw the .zip extension I assumed the "Parts" were somehow attached through the drawing! Whoops...  Does that hold for the Assembly ( Every Part must be attached, and the assembly itself for you to view the drawing of the assembly).  For now, I'll just attach the shaft.prt

Thanks

[MartinHanak · Accepted solution]

Jolene,

INFO: If you want to transport all related data, then create empty directory and use Save a Backup command to save data into it.

Problem info:

drawing ... scale assigned 0.5 ... this is probably your mistake

3 drawing views ... custom scale assigned 1.5

1.5/0.5 = 3 ... this is the reason, why dimension, that duplicates (in AutoCAD) 14.0 receives the value 42.0

Resolution:

Set drawing scale to 1.5.

Note:

3 drawing views ... I suggest to assign drawing scale to them instead of custom scale.

INFO: I used following config.pro options:

DWG_EXPORT_FORMAT	2010
DXF_OUT_DRAWING_SCALE	YES
DXF_OUT_SCALE_VIEWS	NO

MH

[jkmett]

Martin,

It took a couple of days to get around to checking this.  I did find one other problem, maybe its AutoCAD, maybe its Creo.

Using the drawing scale instead of custom provided me with the correct dimensions in AutoCAD, but for some reason the geometry in AutoCAD is using the exported scale, while the dimensions are not.

Example:

drawing scale in Creo: 0.400

Dimension in Creo: 30 in

Export

Dimension in AutoCAD: 30 in

Measurement of dimensions associated geometry in AutoCAD: 0.400*30 = 12

This will actually still be a problem for me, because certain fabricators will (or could) use the AutoCAD drawing directly as a program file in their equipment.

Maybe I'll be contacting AutoCAD at this point?

Thanks!

[MartinHanak]

Jolene,

please ask some AutoCAD expert.

According to AutoCAD Tutorial | Units and Scales | CADTutor AutoCAD drawings are created with scale 1:1 by default. Therefore AutoCAD Measurement tool does not compensate scale value and returns real distance between two drawing entites.

MH

[jkmett]

Martin,

Its more than just the measurement tool.  If I sketch in the exported AutoCAD drawing the imported geometry is scaled by 0.400 relative to any geometry newly sketched in AutoCAD.

Again, thanks for all your help.  I'll get AutoCAD on the line and let them deal with me for a bit.

Thanks and Have a Good Day.

[MartinHanak]

Hi,

please let us know what advice did you receive from Autodesk.

MH

[TrainStopper]

Here we have the settings opposite to Martin!?

dxf_out_drawing_scale no

dxf_out_scale_views yes

For us this seems to work - we routinely make dxf files for sheet metal blanks and they need to be 1:1.

The only glitch we need to be careful about is the first view added to the Creo drawing MUST be scaled based on the drawing scale.

So, where we usually put a 3D default view somewhere in the drawing that might be scaled smaller than the regular views, we are careful to add that 3D view AFTER we have put in a normal view that takes on the default scale for that drawing.

W

[MartinHanak]

This is the right correct answer !