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blad1-Visitor
1-Visitor
October 16, 2013
Solved

ORIGIN 0,0 SETUP IN DRW TO DXF.

  • October 16, 2013
  • 3 replies
  • 6177 views

Hello all,

I am using Creo 2.0 (M030).

We are working in Imperial.

I have all drawing with two sheets. one for all part information and second for machine i.e., scale 1:1.

for machine drawing I want to set origin of part to 0,0. I tried using bellow steps but didn't help.

I select part>RMC>PROPERTIES it opens 'Drawing View'. In Drawing iew I select Origin and set X=0.00 and Y=0.00.

We are exporting all drawings in dxf format. In dxf file while I am checking origin to 0,0 its off on both x and y direction.

Is there any way that I can set origin to 0,0 in creo and while exporting to dxf it remain same??

Thank you for any helpful detail.


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Best answer by blad

It's been long time I raised this question.

I just found solution for this kind of issues. I am sharing it so someone might get help!!!

To get 0,0 ORIGIN in exported DXF from DRW.

1. In model create POINT where you want to make origin 0,0

2. Open DRW file>RMC on part>select "Propeties">in "Drawing View" menu go to "Origin">Check "On Item" in View Origin options> click on "select point" space> select point that you have created on model as Origin point> in "X" and "Y" type 0> Apply> save it and check your exported dxf for 0,0 origin.

Hope this will help somebody. This is solved one of the bigger Issue at my location.

Thnak you.

3 replies

J
JoshH1-Visitor
1-Visitor
October 16, 2013

Hi Brijesh,

usually our programmers have always re-adjusted the DXF as they needed it, so it didn't matter much if the part was turly at 0,0. Our engineers have no clue how manufacturing wants to orient the part, so anything would be a guess.

Since the origin of the format I created is some distances from the bottom left corner, the center of my view ends up on the bottom-left at the orgini of my drawing. By selecting "On Item", I can adjust based on a specific part entity (csys, vertex, etc.).

So...you might want to open the format by itself and turn on the "Location Grid" to see how that compares to what you are expecting for the drawing origin.

Hope that helps a little,

Josh

B
blad1-VisitorAuthor
1-Visitor
October 17, 2013

Appreciated for your quick response.

Just to clarify we have no format for machine drawing (drw) that need to be exported in dxf. It's a blank file with just part geometry on it. and in our company we have automated program that runs design and it creates 100's of dxf everyday for machine to make that sheetmetal part. so if my origin is not 0,0 after exporting in dxf it's not gona work on machine. we cannot open each and every part to adjust origin to 0,0.

Is there any fix for this??

Thanks in advance...

T
TomD.inPDX17-Peridot
17-Peridot
October 17, 2013

Does the program you import the DXF files into not have nesting capabilities?

You might create an "Idea" where you can set a detail.dtl configuration to use the default csys as the view origin. But as far as I know today, there is no way other that some tricks with the geometry to ensure a specified view center by adding a sketched "frame" to lock the view's extent. You might be able to "exclude from export" a particular line type or color. I have not explored this and I don't know if this is acceptable but again, it is the only thing I can think of.

T
TomD.inPDX17-Peridot
17-Peridot
October 16, 2013

I have not had this experience. Remember that the view's 0,0 is not the same as the model's default csys. You can force a view center to be at a specific feature however.

You can confirm the export file's 0,0 by re-importing it into Creo. It could be that a different program assign an arbitrary 0,0, although unlikely.

B
blad1-VisitorAuthorAnswer
1-Visitor
December 9, 2014

It's been long time I raised this question.

I just found solution for this kind of issues. I am sharing it so someone might get help!!!

To get 0,0 ORIGIN in exported DXF from DRW.

1. In model create POINT where you want to make origin 0,0

2. Open DRW file>RMC on part>select "Propeties">in "Drawing View" menu go to "Origin">Check "On Item" in View Origin options> click on "select point" space> select point that you have created on model as Origin point> in "X" and "Y" type 0> Apply> save it and check your exported dxf for 0,0 origin.

Hope this will help somebody. This is solved one of the bigger Issue at my location.

Thnak you.

T
TomD.inPDX17-Peridot
17-Peridot
December 9, 2014

Although I have never been a fan of stray points floating around in my models, this is certainly a good one.

Most of the time I will sneak up on a feature's vertex to get the end of a line or something, but a point does make it easier.

You do have to remember to turn it off somehow so it doesn't become part of your DXF export file. So a layer here is probably the easiest method.

oops... of course, you can use the graphic toolbar's hide-point button,

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