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DXF to AD_PRT conversion


Senior Member
Is there a way to import a DXF so it becomes the 2D drawing on a plane that can then be extruded to the appropriate thickness?

For example the attached drawing. It's a part from a Curliss steam engine model.

Easy enough to import as an AD_DRW and add dimensions to create hardcopy drawing but how to move that into a part.


  • valve disk.dxf
    46.8 KB · Views: 18


Alibre Super User
Hello @jcdammeyer,

- open your DXF as a drawing
- activate sketch
- explode all symbols (in your case the rectangle...)
- goto home screen
- open a new part
- activate a plane for 2D-sketching
and than analyse and repair the sketch, fix all the lines or dimensioning them...
- extrude



Senior Member
Thanks. I repaired the lines in the drawing section first. Then selected all. Didn't realize I could cut and paste between these two programs.

Something else I'm not sure how to do is to reset the 0,0,0 position to a new location. In this case pasting the drawing has it offset to 0. Is there an easy way to move it like it's done in assemblies? Say I want to change the square hole to a round one that is on the same center as the 4 holes which are on a 1.375 pitch diameter. And I want that at 0,0,0.

Just to add to this. I can move individual parts which can get tedious or even change the shape of the part. But to select the whole works and make one point the 0,0 location. Is there a quick way?
Last edited:


Alibre Super User
Say I want to change the square hole to a round
For example it coud be done in the drawing:

- choose Point in the drawing menu:


- select the crossing lines:


-select eg circle from the menu and draw a circle


- delete crossing lines and the rectangle

- change to part sketch
- repair...
- Select Move
- Select all figures you want to move


- select "From"
- select the center of the circle

- then selet "to"
- then select the Origin of your sketch


- press apply



Senior Member
For example it coud be done in the drawing:

- choose Point in the drawing menu:

- press apply

Thank you. That was the hint I needed.
I did it in the part editor.
1. First edit the sketch.
2. Place a Sketch Node in the middle of the square. A faint red line appears showing it lines up with the top hole.
3. Select Dimension flyout and set it to 0.75" which is proper distance from the PDF drawings I have.
4. Now drag a box around all the parts to select everything.
5. And then select the Move dialog under the Sketch Menu. This is where I was always confused.
5a. The figures are already selected so I can ignore the first box.
5b. Click the 'from' box, it highlights, and click on that Sketch Node I created in step 2.
5c. Now click on the 'to' box and then move the cursor over the 0,0 position and click.
5d. The Apply button is made active and can be clicked which moves the part.

When I write Delphi Windows applications I always try and create as many hints as possible when a mouse hovers over something. Unfortunately that move dialog doesn't have that done so it's just that little bit harder to use. Having written the procedure above I think I'll remember it now.



Senior Member
Oh and just to show what I've been playing with and trying to decide if I want to go down the rabbit hole and build one you can see where that little valve disk goes.

The builder has a couple of videos here:



Staff member
Also consider getting familiar with the Copy with Base Point and Paste Stamper commands.

You can for example choose which node of your sketch you want to act as the "zero" point, and then use the paste stamper to paste the figures right on the origin. This can make this kind of operation much simpler.


Senior Member
Followed the directions in that link. Activated 2D sketch. Put a point in the middle of the small box to serve as the base point. Select all works.

And I can copy and paste into a new part. But as the screen shot shows, there is no copy with base point enabled.

And since the menu entry is disabled it's likely even a hint would show up as to why it isn't enabled.


  • AlibreNoCopyWithBasePoint.jpg
    71.7 KB · Views: 10


Senior Member
You can't select anything if it isn't.
Process is.
Import DXF file.
Activate 2D Sketch and a red lined box surrounds the drawing.
Select All and the lines inside the red lined box turn blue.
At this point you can control-C or select copy from the menu.
Create new part drawing.
Select Plane and activate 2D sketch
Control-v which then also brings up the explode custom objects warning.

Doesn't matter if the square box in the middle (with the X lines) is there or not. Try it. The DXF is at the beginning of this thread.


Alibre Super User
And I can copy and paste into a new part. But as the screen shot shows, there is no copy with base point enabled.
On my computer in the drawing workspace the icon for Copy with Base point is greyed out and the option is not selectable.

See - no highlight with the mouse over the command.
Cop wBP Dwg WS.png

But it is selectable in sketch mode of the Part workspace even though the icon is greyed out. And when selected it asks me to select a point. Odd behavior. :confused:

The command is highlighted with the mouse over it but since the icon is greyed out it may give the impression that it is not available. (Also note the Copy icon in both screen shots.)
Cop wBP Part WS.png


Alibre Super User
Staff member
Odd - copy with base point works from a new empty 2D drawing into which I sketch a few features on sheet.

I see no obvious reason why an import from DXF should change the behaviour.


New Member
Not that it helps much but I found that if you assign a drawing template to the opened drawing of the dxf then the copy with basepoint is accessible.


Senior Member
Yes that does work but the part is not completely inside the drawing template and I haven't figured out how to move it. Cut and paste it a number of times deleting the pasted item each time has it move up diagonally until it is inside the template. And then it can be selected with base point. Even asks for the base point. Try placing that in a part drawing though and it doesn't appear to work. But I'm probably doing something wrong there.


Alibre Super User
Yes that does work but the part is not completely inside the drawing template and I haven't figured out how to move it.
That's not needed :)
If you have assigned a drawing template (doesn't matter which) you drawing maybe looks like this:
The part is not in the range of the paper...
Ignore it.
- activate the sketch
- explode the symbol as before
- set a point eg. at the crossing of the two lines
- drag a rectangle around the part
- select copy with base point
- select your point
- go to your 3D-part
- active a sketch
- choose paste stamper
- choose eg. origin

Hope it helps



Senior Member
I hope that it's OK to attach my "issue" to this post as it's at least relevant for the "repairing" of the subsequent part.

I did some metal artwork back in 2003 in another 3D tool (Ashlar Vellum), and I now want to import and create these as parts in Alibre.

I have done all the above instructions and do get a 2D image on a sketch. I also get a warning about copying custom symbols which I don't think that I have, and I promptly ignore the warning and do the copy anyway.

The ensuing 2D image looks perfect to the eye, but when trying to exit, I get the dreaded message that the image isn't closed. Well, I will fix it by removing a few lines and replacing them with some that interconnect properly, except I can't get my select tool to recognize the line ends that I want to use to close the figure.

I'm trying to safeguard my art design(s) as I don't want to pay "the other" toolmaker yearly fees when I have decided to use Alibre.

Any resolution to this issue will be greatly appreciated.




  • Gazer 1 Hole 20.dxf
    83.3 KB · Views: 5


Alibre Super User
Each line segment was its own custom symbol, so Alibre was seeing them as not part of the sketch.

I exploded each "custom symbol", leaving just the line segments and it now shows as a closed loop.

Try this file:

just to verify, I pasted it into a sketch and extruded it into a solid. I had to delete the dimension first, as Alibre wasn't liking the imported dimension.



  • Gazer 1 Hole 20.AD_DRW
    739.5 KB · Views: 3


Senior Member
It certainly works!!! but I have no idea of how you did/mean with this operation:

"I exploded each "custom symbol", leaving just the line segments, and it now shows as a closed loop."




Alibre Super User
Right click each line segment, and select "explode". For some reason, somehow, each of your line segments imported as a seperate symbol. So you have to explode each and every one. Like, 4 or 5 total. I don't remember exactly how many there were.



After exploding all of the line segments, I hit "analyze sketch", which showed pretty clearly an open loop.

I also deleted your dimensions. The imported DXF dimensions imported strangely into Alibre when I tried to extrude earlier. It threw errors until I deleted them.


I used the intersect tool to close the open loop.


Then the trim tool to clear the excess.


Now, the "analyze sketch" tool shows that everything is good-2-go.


Now, all is ready for copying, pasting, extruding, etc.

I hope this helps.