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Problem Importing DXF file in SW2008 SP 4.0 - but no Problem with SW 2
2

Problem Importing DXF file in SW2008 SP 4.0 - but no Problem with SW 2

Problem Importing DXF file in SW2008 SP 4.0 - but no Problem with SW 2

(OP)
I am importing the same dxf file in SW2007 and 2008SP 4.0

In 2007, the dxf file comes in with a series of circular arcs forming a fully closed ring that can be extruded.

In 2008, instead of coming in as a series of circular arcs, I get multiple blocks to fully form the ring, but when I go to extrude it, it tells me that there is an open loop somewhere.

When I check the 1st block I find that the symetry is correct to 8 displayed decimal places so that the 2nd block should be able to link perfectly on top of the 1st one and so on.

I have 2 questions:

1)  is there a way to prevent the dxf file from automaticaly coming in as blocks in SW 2008
2)  How do i correct for closing the loop when blocks are used and each block looks ok from a symetry point of view?

 

RE: Problem Importing DXF file in SW2008 SP 4.0 - but no Problem with SW 2

(OP)
I have further discovered that when I remove all but one of the blocks and then connect the end points, I still cannot extude it without an error saying that there is either more than 1 closed loop or an open loop.  When I checked the endpoints, everything is properly connected.

Any ideas on how to close the profile without redrawing by hand?

RE: Problem Importing DXF file in SW2008 SP 4.0 - but no Problem with SW 2

Can you post the DXF file for testing?

cheers

RE: Problem Importing DXF file in SW2008 SP 4.0 - but no Problem with SW 2

How are you getting the DXF into SW?  Rather than open it in SW, I typically open the DXF (in DWGEditor) and copy it and then start a new sketch and paste it in there.   

Flores

RE: Problem Importing DXF file in SW2008 SP 4.0 - but no Problem with SW 2

(OP)
File Open  

Select a DXF file

Select as a new part

click finish

then click on extude

in 2007 it extrudes - in 2008 it does not

RE: Problem Importing DXF file in SW2008 SP 4.0 - but no Problem with SW 2

The sketch is full of open contours. They need to be fixed before you can extrude.

Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 08
ctopher's home (updated Aug 5, 2008)
ctopher's blog
SolidWorks Legion

RE: Problem Importing DXF file in SW2008 SP 4.0 - but no Problem with SW 2

Don't try to directly import a DXF with blocks.

Open the file with DWGEditor first and explode all the blocks.  Otherwise, SW can't merge points.  In order for two lines to be joined in SW, they have to share the same point.  Not be at the same point, but the same point entity must be the endpoint of both lines.  If points are "contained" inside blocks then they can't be merged.  

-handleman, CSWP (The new, easy test)

RE: Problem Importing DXF file in SW2008 SP 4.0 - but no Problem with SW 2

Open the DXF into SW.
Edit the sketch and delete all but one of the blocks.
Explode that block.
Close the sketch.
Start new sketch and create a circle using the origin and the two free end points of the tooth profile, and extrude to create the body of the gear.
Create new sketch and convert the tooth profile entities, and extrude to create a solid tooth.
Pattern that tooth.

A much simpler alternative is to download a solid gear from Boston Gears or similar.

cheers

RE: Problem Importing DXF file in SW2008 SP 4.0 - but no Problem with SW 2

(OP)
CorBlimeyLimey

These dxf files are accurate enough to make master gears out of which is not the case with anything from Boston Gear or from Gear Trax.

If these are open contours, then how did SW2007 and previous version close them?

RE: Problem Importing DXF file in SW2008 SP 4.0 - but no Problem with SW 2

You will have to do what CBL suggests.
I opened it in AutoCAD 2008, exploded the blocks, there were still open contours...even in ACAD.

Was it the same file used in SW 07? Were there changes with the file in ACAD lately?

If it is the same file, then maybe SW 08 has been updated to be more sensitive than 07 and catches the error easier.

Chris
SolidWorks/PDMWorks 08 3.1
AutoCAD 08
ctopher's home (updated Aug 5, 2008)
ctopher's blog
SolidWorks Legion

RE: Problem Importing DXF file in SW2008 SP 4.0 - but no Problem with SW 2

It sounds like SW 07 didn't import the DXF blocks as SW blocks.  Since it's not importing the blocks as blocks but individual entities, the "merge points" in the import will merge any two points that are within the tolerance.  I think the tolerance defaults to 0.001.  When it imports blocks, it can't merge two points from different blocks into a single entity, because each block has to have its own point.  It takes like 10 seconds to open the file in DWGEditor, type in "explode", and pick "select all" or whatever from the popup menu, then save the file as DXF again.  All entities will then import as separate sketch entities and the "merge points" will form a continuous profile.


 

-handleman, CSWP (The new, easy test)

RE: Problem Importing DXF file in SW2008 SP 4.0 - but no Problem with SW 2

That would definitely be quicker, but creates a lot more unconstrained sketch entities.

If the import blocks via dxf is new to SW08, perhaps an ER for the ability to choose is in order.

cheers

RE: Problem Importing DXF file in SW2008 SP 4.0 - but no Problem with SW 2

(OP)
ctopher  The exact same file opens and extrudes fine in 2007 but not 2008.  

Handleman  - I think that you are correct that SW07 did not use blocks and therefore the merge points defaulting to .001 worked.  I also noticed that changng this sensitivity does not work in SW08  - probably because of the blocks.

I have tried your method of exploding the blocks in the drawing editor and it works well.

I further tested the theory of the blocks by bringing in the original dxf file into SW08 as I did originally.  I selected all of the blocks and exploded them.  The profile did not extrude.

In another test, i imported the dxf file in the original manner and then deleted all but one of the blocks.  I then drew a line to close the endpoints of the blocks to see if it would extrude.  It did not extrude.

I then selected the block and exploded it leaving the line I drew to close the profile in place.  It still did not extrude.

I then deleted the line and redrew it to the same endpoints.  This time it did extrude.

This tells me that it is definitely related to the endpoints in the blocks that SW08 created that do not allow them to merge.

CBL is correct that the SW people need to be made aware of this to allow someone to choose how to open the dxf file, or have the system be more forging like SW07 How does one do that in an effective manner?  Maybe CBL has an in?

This particular dxf file was created within the genaral dxf file standards so it seems that if SW is going to read in a DXF file, its should be forgiving enough when something is within that standard.

RE: Problem Importing DXF file in SW2008 SP 4.0 - but no Problem with SW 2

Just use the Enhancement Request function at the SW portal.
I just did so under the Import/Export > DXF/DWG > Blocks category ---> "Offer a choice of importing blocks or sketch entities when opening DXFs"

You could also post the ER for support in the SW discussion forum at http://forum.solidworks.com/

The more ERs received the higher the probability of the ER being implemented.

cheers

RE: Problem Importing DXF file in SW2008 SP 4.0 - but no Problem with SW 2

(OP)
All

I have notified Solidworks of this issue and they are in agreement that this needs to be resolved - they have issued Service Request # 1-973216802 to this issue

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