Problems inserting blocks

I'm currently using sw2007 sp2.2. I am haveing a probleminserting 2d blocks into a drawing.

I am trying to add a pnematic schematic to the drawing. howeverevery time i try to insert a block containing a valve, or FRL, ect.solidworks inserts my revision block instead of what is containedin block file.

Does anyone have an idea where to start?SolidworksWorkgroup Pdm
Comments 13
TS
TS 2013-07-22

I've got a similar problem Nancy had in 2009.

I also had the same problem back in SW 2008 of which there was no solution other then to not use SW.

The problem still exists in 2013 and I now need a solution.

I'm creating a drawing and need to insert blocks.

Every time I insert a block SW decides to add some text to the block.

I've created blocks from SW drawing views and then inserted them into a new drawing.

I've create a sketch of a circle in a blank SW drawing, saved it as a DXF file.  Then inserted it into a new blank drawing and SW decides to add some text.

I've create a square in Draftsight, saved it as a dxf file, then inserted in into a blank SW drawing file.  SW decides to add some text.

The text inserted is not random.  It's 2 notes that we use on most of our drawing templates

TS
TS 2013-07-22

video attached

JB
JB 2013-07-22

Good video Tom.

I noticed you were working in the sheet format.

What happens if you insert the block into the regular drawing sheet?  Does it still pick up your notes?

TS
TS 2013-07-22

Notes are picked up in either, in the sheet or on the sheet.

I have tried a couple of  solidworks blocks and it does not pick up the note.  DXF or DWG are the only things effected.

AW
AW 2013-07-22

In the dxf files are your purging the files before you bring not SW.  Tree is no extra fluff in the dxf's.

Can you post a dxf file you would like to make into a block or SW block file for us to try?

Cheers,

Anna

TS
TS 2013-07-22

test.dwg was created in DraftSight and the file from the video

circle.dxf was created in a SW drawing.  when reinserted text is added

Both the HE-0642 files were created from a SW model.

This assembly is modeled.  I created a drawing view, then saved the drawing as a dwg.  Bringing it into another SW drawing as a block adds the text.

Before you ask why...

I'm triing to creat an elevation drawing between several large machines.  Some are modeled some are not.  SW may struggle to open all files together anyhow.

Making an elevation view of each machine from what ever software it was done in I can piece them all together in a SW drawing to create my production line elevation drawing.

TS
TS 2013-07-22

I did not think to use the purge as some of these files are created by SW and the test files were new draftsight files.

AW
AW 2013-07-22

Draftsight has a command called Clean.  I think you can find it under File.

Purge also works.  That is what I use in the command line.

Cheers,

Anna

JB
JB 2013-07-22

That's interesting.  I've noticed this occuring on occasion when I insert a DWG as a block.  In my case, I usually explode the block, delete the extra crud and reblock it. 

Let me ask, before inserting the block are you removing from the solidWorks drawing block definitions that aren't used?  (They'll appear in the blocks folder kind of ghosted.)

Here's my hypothesis:

If a drawing has a block definition called "Block1" of an annotation that previously had attributes, then SolidWorks created an annotation and and attached it to the block insertion.  That annotation was called Note 1 and SolidWorks associated it with the insert as it's attribute text (AutoCAD does something similar)  When that block insertion was removed and the definition left behind the note assigned to it was deleted but not the fact that the first insert of "Block1" has Note1 attached to it.  So now, you insert an AutoCAD drawing which reguardless of what the AutoCAD drawing is called, is called Block1.  SolidWorks creates the insert and says, "Hey note1 goes with this)  Well, note was was deleted and so your general notes became note1 and SolidWorks attaches them to the block insert.  If this is the case, you should be able to turn off the notes by turning off the display of attributes for the block insert (you do that from Property manager with the block insert selected.)

That's just a test.  The solution in this case is to delete the existing definition of "block1" from the blocks folder and see what you get when you insert your DWG into the drawing.

In any case, I would report this to your VAR and open an SPR to get it fixed.

Finaly, can you post the DWG you created so we can check it out and be sure it's not carrying any unintended baggage-maybe in the template itself?

TS
TS 2013-07-22

I think I understand what you're saying John.  Kind of like how SW handled deleted calculated dimensions.  If you delete a dimension with a calculation the next dimension you put in get the alod calculation.

Going into the property manager of the block shows some of the text in the attribute section.  Not all of it.

How can I generate a new, clean, empty template?

template, block and resault file attacked.

JB
JB 2013-07-22

OK, Tom.  It looks like the DXF comes in with the attributes in that drawing only.  Your template seems to be clean.

Even that drawing isn'ta  total wash.  If you delete the block definition and re-insert the dxf, it looks like it comes in without the attributes.

To delete the block definition:

You can also edit the definition of the block and delete the attributes and they stay gone in subsequent insert operations.

I tested this on 2013 SP4.0EV.

TS
TS 2013-07-24

Thanks for the work John.

My VAR should be sending this to SW.

I've been editing each block as in insert them.

SW is not making my job any eaisier.

TS
TS 2013-07-25

Here's my solution.

After resetting my registry setting the problem was fixed.

As I started to add my preferences under "Tool, Options" the problem came back.

When I select one of my drawing tempaltes under "Default Temapltes" the problem appears again.

If I select one of the SW default tempaltes the problem goes away.

Resetting the registry leaves the "Default Tempaltes" blank.  This works too.

Another problem SW should fix.  There is a "Reset" button on the "Tools, Option" pages.  This button does not reset the default tempaltes page.  It clears the fields while you're looking at the page but closing and reopening the form brings the old values back.  Thank SW!