imported dxf file is x10 scaled

[Anonymous]

I export a PCB from Eagle CAD as a .dxf file. I don't have much option there just select in mm scale. (dimensions are 33x34 mm)

Then I import it to Fusion 360. However, it is imported as x10 scale (330x340 mm)

I can decrease it x10. I want to follow the sketch to create 3D model of the PCB. When I click on sketch property, it automatically goes to its original dimensions (330x340 mm).

First of all, why is it scaled x10 when dxf is imported? There is almost no configuration option but do I import it wrong or could it be a case that Eagle Cad generate .dxf file wrong?

How can I keep the re-scale dimension when I click on scale-rectangle option so that I can use the sketch as a reference?

[FrankCao]

Hi serdar,

Thanks for letting us know the issue. Could you help attach your dxf file here for us to do some analysis?

There are two ways of import dxf into Fusion. One is upload it using the data panel( You can click "upload" button on side panel and upload your dxf file to the cloud, then open it after upload is finished), the other ways is directly insert it into sketch.(We have “Insert --> Insert DXF” command to help you do this)

Did you see the problem by both ways? Or you only see the problem from one way?

Thanks,

Frank

[fangfr]

Hi @Anonymous,

Fusion have two ways to import DXF file. One is Upload on the data panel. The other is Insert DXF command. Which way are you using? Could you please post your DXF file here? Thank you. 

[Anonymous]

Hi Frank and fangfr,

Thanks for the answer. I tried the both way to import the dxf but the result is the same, x10 scaled drawing.

I think a setting in my Fusion 360 should be importing .dxf with x10 scale.

 I download a .dxf file from Panasonic https://www3.panasonic.biz/ac/ae/dl/cad/index.jsp?series_cd=2481&part_no=EKMC1603111

Its datasheet defines the diameter as 22 mm. But, what I see is 220 mm in Fusion 360.

What should be the next step to diagnose the problem?

[fangfr]

Hi @Anonymous,

Thank you let's know this.

I have downloaded that DXF file from Panasonic website. Could you please check if it (ekmc160311 copy.dxf) is the same with the one you saw? Thank you. The DXF file does not include the units information. In this case, Fusion will give it a default units. So, you are seeing 200 mm. 

[Anonymous]

Hi Fangfr,

Yes, it is the same file that I import:

 

Do you see the diameter 22 mm or 220 mm?

[Anonymous]

Preferences shows that it uses mm as unit and I couldn't see any default scale option

[HughesTooling]

Unfortunately Fusion defaults to CM when there's no unit info in files there have been several request it default to the document units but so far no update. So what you're seeing is Fusion is importing the file as 20cm then converting to 200mm.

Mark

[Anonymous]

I select all layers then use Modify > Scale > 0.1 scale factor that sets the drawing to its original dimensions. However, when I press R button and click on the drawing, it immediately scales x10 again.  How can I solve the problem?

I tried to save x0.1 drawing as IGES, then import it to a new project, but then I can't see the drawing in the new project.

[HughesTooling · Accepted solution]

You can only import curves with DWG\DXF files. The reason the sketch resizes when you edit it is because the edit rolls the timeline back to before the scale. Do you have any other programs you could scale the dxf down before you open it with Fusion.

Mark

[Anonymous]

Thanks for the explanation. I have QCAD that never used before. It would be more convinient to solve the problem wiht Fusion 360 if it is possible as I will be importing some many components and PCBs.

Is there a way to merge time line after the rescaling or prevent (lock) the lime line to go back?

EDIT: Scaling in QCAD was very easy and now I am able to use the drawings correctly. However, it would be good to know if there is any way to solve it with Fusion 360.

[HughesTooling]

Nothing is going to work too well, one option is to start another sketch after the scale feature and project the scaled down sketch into it. Another option would be to work without history.

If you could import all the DXF files into another program scale them down and put each one on a different layer when you insert them each one will generate a sketch so you could do a batch import that way.

Mark

[Anonymous]

I have found a solution to this. I was having the same issue with files created in AutoCad and then importing into Fusion. I now open the dxf in Draftsight and set the units to Milimeters and re-save. This then imports into fusion at the right size. Perhaps there is a way to do this in AutoCad, but i'm using dxf's from a colleaue and I don't hace Autocad.

[Anonymous]

Hi,

I experience the same problem with my DXF files.

I wonder why the default import scale is cm. It is rarely used as a unit in professional design work, as I understand it. Millimeters is a much more commonly used a measure when designing items.

Please add a option to override units when uploading DXF files.

Or, why not just use the already preferred default design unit. It's there and it's should be usable, instead of the hardcoded cm unit in the DXF import code.

Regards..

[Anonymous]

I just tested how to edit the DXF file to set the units before importing it to ADF360.

First I tried editing the $DIMSCALE which specifies an overall scaling factor. The value in my DXF file was 1.0, so I set it to 0.1, but that has no effect. It seems that ADF360 does not respect that value. Maybe there are rules to when this scale is used, so I made another attempt.

I edited my file to include this setting in the header, which was missing from my file:

$INSUNITS
70
4
9

And that did the trick. 4 is the magic number which means millimeters.

I used PSPad to edit my file on Windows10. DXF is just a text file, so you can edit it if you just keep the format. I did not try editing with Notepad.

[Anonymous]

Hi Guys,

One of our customers had the same problem. The eayest way to fix this witout opening any 3rd party app or AutoCAD is that you do not upload the dxf to your folder, but IMPORT it to a specified plane. During the insert it you can set the units to mm. Hope that helps!

[harry.doldersum]

@Anonymous 

Thanks, this tip was a great help! 😎

[Prometeuszu]

Year 2024 and still same problems! Great support.

[etfrench]

Fusion's behaviour when importing unitless files is well documented.  What is your issue?

[spsie]

This is the answer I was looking for.  A good solution.