DXF/DWG Export Layers not representative of Creo Layers

[M_C_Anderson]

I am trying to wrap my head around how layers are handled when exporting a drawing to a DXF or DWG. I have already discovered the issue where you cannot have the same entity on multiple layers, since the export will only place it on the first alphabetic layer that it appears on. However, I am struggling to get all the exported layers to accurately represent the ones in my Creo Parametric files.

In my case, I have a number of sketches for a soft goods flat pattern. Each type of sketch (outlines, folds, seams, etc.) are assigned to their own layer. Those layers are then mapped to identically named layers in the export settings. The results, however, are inconsistent at best. While some of the exported layers do contain the correct items, many of the items simply get placed on a new layer named "0", and cannot be controlled by their original Creo layers. I cannot for the life of me see why this is the case.

Does anyone here have experience with DXF/DWG exports, and could offer advice on ensuring the exported entities retain their original layer? 

[MartinHanak]

Hi,

my suggestion:

• in Creo assign a unique color to entities that belong to a certain group
• export DXF/DWG from Creo
• open DXF/DWG in AutoCAD (full edition) and create layers in it ... use unique color to select layer entities
  • I hope you can automate this process by creating LISP script

[M_C_Anderson]

I appreciate the input, but this is unfortunately not a good solution for our team. We already have a standard in place for entity colors, line fonts, and layers. We also can't use AutoCAD in addition to Creo for every one of our engineering releases. 

We should be able to assign layers in Creo Parametric, export those layers to DXF/DWG, and get the layers we expect in the export file. If Creo Parametric is incapable of doing so, then a ticket needs to be opened and PTC needs to fix this.

[M_C_Anderson · Accepted solution]

I found out a bit more what is happening. I have multiple UDF groups that create sets of sketches. The layer that gathers these sketches is rule-based, and looks for those groups based on their name. Since the UDF cannot re-use sketch names, it names the sketches inside the groups after the first the generic "Sketch #" name, which is not gathered directly by the rule.

So, even though the layer is working in Creo Parametric, it is only doing so by way of the group. I believe for this to work fully, I need to come up with a way to have the sketch features inside those groups directly gathered by the rules, since I cannot rely on the group layer rule for the DXF/DWG export layers.

Update: Alright, I found that by changing my rule from looking for ["curve features" by "curve features"] to ["features" by "group"], I am getting the desired results. I'll make sure from here on that all our layers are gathering the features explicitly, rather than relying on their group.