Export selected as dxf in drawing

[safiredesignengineers]

Hi group

I normally export my dxf's out in the 3d mode and use export face as...

Is it possible to export out in drawing mode so that only the selected item is exported out as a dxf with the standard options for version etc..?

It would be great to do this, sometimes after a model has been created it is necessary to add some bits to the exported dxf for manufacturing purposes which get removed during manufacture, so they are not actually part of the model.

we get around this in different ways.

But to be able to export from the drawing view just the selected item will mean we can add sketches with the bits we need, which is not connected to the actual model, then simply export the select item as a dxf. 

is this possible?

Regards Adrian

[safiredesignengineers]

Hi Group

Any feedback on this?  I use Rhino a lot and with Rhino you can select anything on the screen and export out individually as a dxf. This can be anything from a single segment to the whole drawing.

I would like to be able to do this in inventor drawing mode. At the moment the only way I can see to get a full scale dxf is to use "save as" and then save as a dxf, but it will only export the whole page?

Is there a better way? Or is this going to be updated?

Regards Adrian

[bobvdd]

Inventor's IDW does not have the notion of selective export (except for sheets and removing the title block).

Did you ever explore Inventor DWG instead of Inventor IDW format?
This would avoid the export phase and would allow you to experiment with different additional sketches or draft views and immediately see the result in AutoCAD.

The other suggestion I have is to use the "Suppress" command on the views you temporarily don't want to see in the DWG.

Bob

[safiredesignengineers]

Hi Bob

I use the DWG drawings as my main choice in inventor but due to various limitations I tend to use Rhino as a work horse for certain things.

I don't really use autocad, for one it takes too long to load up and Rhino loads in a flash.

I need to work with dxf's as opposed to dwg's as my machines and other software understands them better.

I would actually like to do everything in inventor as opposed to using different packages but this is not possible as there are limitations to it. In this particular area with rhino I have an infinite space as opposed to a drawing sheet and it doesn't matter if my part is small or large I can whiz round the screen and go into 3d etc.. Very quickly and efficiently.

However If I were able to export a dxf out of a selected item at full scale regardless of the scale in the drawing this would change things considerably and make life better and easier within inventor.

Perhaps this is an area to add to the wish list?

Regards Adrian

[bobvdd]

Sure I could enter a wish but I would much rather like to help you today and find out if we could do a slight adjustement to your workflow to make it work.

Another thought (let's assume you have a single sheet IDW):

1. Create a second sheet and Copy/Paste  the view you want to work on on that second sheet
2. Use the Crop command on Sheet:2 to extract the portion of the design you want to highlight
3. Save Copy as DXF and use an ini configuration ini file that exports only Sheet 2 at full scale modelspace

 

The use of the ini file should considerably speed up the process.

Might not be as smooth as in Rhino but it might work for you.

Bob

[safiredesignengineers]

Hi Bob

this works to a point and should be handy, however I have found an issue:

I want to be able to add and sketch extra bits then export. I just tried this and I can't seem to export my sketched extras?

regards Adrian

[bobvdd]

What if you do this:

1. Create a second sheet and Copy/Paste  the view you want to work on on that second sheet
2. Remove border and title block on the second sheet.
3. Use the Crop command on Sheet:2 to extract the portion of the design you want to highlight
4. Scale the cropped view to 1:1
5. Save Copy as DXF and use following options (uncheck "Use model geometry only" and "Base View Scale - Model space")

Cheers

Bob

[safiredesignengineers]

Hi Bob, that works but I then have to scale 1:1 and some parts can be big so I then have page size issues.

What we need is a simple export selected function so that is exports selected items at 100%.

Another thing I noticed was:

I need to add things like tabs onto sheet metal parts for various reasons, so I select my view, go to sketch, then project lines etc.. All works well but the projected lines are not really editable i.e if I had a circle on my drawing and I wanted to add a tab I would select the view, go into sketch. Project the circle, I would then drop a rectangle on it that is dimension for my tab and then I would want to trim the rectangle and circle so that I end up with one profile. The rectangle is no issue the circle can't be trimmed, I can drop another circle on top of the projected circle and trim this, but when I then export I end up exporting the original circle and the trimmed circle.

This is all a bit messy, clumsy and long winded.

I think inventor needs a few new features to make it more usable in general but for manufacturing we could do with a few tools on the 2d side to work on profiles and flat patterns, without having to go into auto cad (or in my case Rhino)

Is this an area that will be developed?

Regards Adrian

[bobvdd]

If your view is larger than your sheet it will still export correctly I think.

Besides you can always define custom sheet formats that fit your large scale views  🙂

\

To your second point about projected geometry that cannot be trimmed. Circles can be tricky at times.

Theoretically you should be able to use the "Break Link" context menu to give yourself  the opportunity to trim the circle rather than duplicating the arc.

If break link menu is not there, try "Select other..." to select the curve instead of the edge.

If that still does not work, use the "Select as edges" + "Visibility" menus on the view to make the circular hole temporariliy invisible in the view and to be able to select the projected curve  for  the "Break link" operation without ambiguity.

Bob

[safiredesignengineers]

hi Bob

where do i find the break link option if it was there?

Rgds Adrian

[bobvdd]

RMB on your projected circle and then see snapshot.

Cheers

Bob

[bobvdd]

Window selecting the circle might also help to get access to the "Break link" functionality.

At any rate there is something funky going on with breaking projected geometry in certain projected views, so I logged a defect

1409307 Cannot break link of projected geometry in certain projected views

Thanks.

Bob

[safiredesignengineers]

Hi Bob

I have got the break link working and I will try to use this in my work flow. What we really need is more functionality in the 2d and 2d drafting side, really autocad should be integrated into inventor so it works really fast and smooth as one product.

One day it will have to combine as people won't be using standard autocad as the 3d develops more.

Regards Adrian

[bobvdd]

I cannot argue with that :-).

Bob

[wobke11]

I know this is a very old thread but this is exactly what I need to find so hopefully you are still active and able to help me

---

@bobvdd wrote:

Sure I could enter a wish but I would much rather like to help you today and find out if we could do a slight adjustement to your workflow to make it work.

Another thought (let's assume you have a single sheet IDW):

1. Create a second sheet and Copy/Paste  the view you want to work on on that second sheet
2. Use the Crop command on Sheet:2 to extract the portion of the design you want to highlight
3. Save Copy as DXF and use an ini configuration ini file that exports only Sheet 2 at full scale modelspace

 

The use of the ini file should considerably speed up the process.

Might not be as smooth as in Rhino but it might work for you.

Bob

---

How would I edit my .ini file to scale the DXF to full scale (1:1)?

I currently have:

[EXPORT SELECT OPTIONS]
AUTOCAD VERSION=AutoCAD 2000
CREATE AUTOCAD MECHANICAL=No
USE TRANSMITTAL=Yes
USE CUSTOMIZE=No

CREATE LAYER GROUP=No
PARTS ONLY=No
[EXPORT PROPERTIES]
SELECTED PROPERTIES=
[EXPORT DESTINATION]
SPACE=Model
SCALING=GEOMETRY
MAPPING=MapsBest
MODEL GEOMETRY ONLY=Yes
EXPLODE DIMENSIONS=No
SYMBOLS ARE BLOCKED=Yes
AUTOCAD TEMPLATE=
DESTINATION DXF=Yes
[EXPORT LINE TYPE & LINE SCALE]
LINE TYPE FILE=COMPATIBILITY\Support\invANSI.lin
Continuous=Continuous;0.
Dashed=DASHED;0.
Dashed Space=DASHED_SPACE;0.
Long Dash Dotted=LONG_DASH_DOTTED;0.
Long Dash Double Dot=LONG_DASH_DOUBLE_DOT;0.
Long Dash Triple Dot=LONG_DASH_TRIPLE_DOT;0.
Dotted=DOTTED;0.
Chain=CHAIN;0.
Double Dash Chain=DOUBLE_DASH_CHAIN;0.
Dash Double Dot=DASH_DOUBLE_DOT;0.
Dash Dot=DASH_DOT;0.
Double Dash Dot=DOUBLE_DASH_DOT;0.
Double Dash Double Dot=DOUBLE_DASH_DOUBLE_DOT;0.
Dash Triple Dot=DASH_TRIPLE_DOT;0.
Double Dash Triple Dot=DOUBLE_DASH_TRIPLE_DOT;0.

But I have no clue what to put there

[wobke11]

Nevermind that, I have since figured out you can create an ini file automatically from settings you define