Make Drawing From Part Issue

[ClockMaster]

I am hoping some of the SolidWorks Guru's can help. I am trying to make a simple drawing from a basic part created in SolidWorks. I want to make a .dxf in a 1:1 scale. I have set the document properties to ips and changed every setting to inch that I could find even under the save menu. Me nor my professor can seem to get it to save a .dxf in inches. I am using the 2008 version on my college's computers. If someone could list the steps to get a drawing in inches I would appreciate it.

[mcphill]

Can you post the file? The steps will depend on the settings in the file. I can give it a whirl, get the DXF for you, and then tell you how I got there, but I need the file to do that.

[JerryFlyGuy]

There is actually a detailed step by step proceedure for doing this already posted here at cnczone.. [I'd have to do a search for the post..]

The basic steps are:
1- Model the part
2- Creat new file> drawing [select whatever template you want.. don't worry if the part is larger than the sheet when it's 1:1
3- insert the part onto the drawing sheet.
4- Save drawing as a solidworks drawing.
5- Save-as use the button & down @ btm of Save-as window to select dxf or dwg and save the file.

Note this will produce a 2d drawing only.. you cannot save a 3d dxf from Solidworks..

Fwiw

J

[broby]

If you create the part in Inches and then insert the part into a drawing sheet like Jerry states, you will be able to save-as the file as a imperial sized DXF.
Make sure you set the drawing scale at 1:1 before exporting the file as a DXF otherwise your DXF file will be the wrong size.
Cheers
Brian.

[JerryFlyGuy]

DWG from a solid file

Is one of my orginal [or at least earlier] posts on this subject w/ a bit more of a complete description..

Does this work Clockmaster?

<edit> Also forgot to note that when doing this proceedure it's recommended to add at least 1 dim per part as a 'check dim'. This ensures that you can confirm the part scale in Acad. Sometimes when you re-measure the part in Acad the dim will be scaled [not the part] so you need to go into the dim format manager [can't remember the exact name of it, I use it regularly but just haven't stopped to look at it in a while ] and make sure that the dim scale is 1 [under the precision tab?? I think]

Fwiw

J

[ClockMaster]

I am in the lab today I will try out those steps and post results. Here are some of the parts that I drew. Also all the defauly sheets format are in mm does that matter?

Update....Followed all the steps and the dxf is still in SI units. I wish there as a simple switch to set SolidWorks to between Imperial and SI.

For the drawing I went to Tools Options Document Properties and for Units selected IPS with decimals of .1234. The drawing came out correct with Smart Dimension using all inches. I saved the part and then went to File Make Drawing From Part.

From here I notice that all the Sheet Formats are in mm's
I pressed cancel then went to Tools Options Document Properties and for Units selected IPS with decimals of .1234
Then I right click on sheet1 in the left fram and go to properties.
Select Standard sheet size bubble and there all in inches.
I picked D-Landscape and unchecked Display sheet size
At the top for Scale I made it 1:1
I then saved it as a .slddrw and then again as a .dxf
And finally its in inches.

[broby]

I noticed that you did not "Tie" your sketch to the "Origin" point in each part.
Whilst your sketch is "Fully Defined" within itself, i.e. all features can not move in relation to any other feature, the whole feature can move.
If you set a Relationship between the origin and some point on your sketch, you will see things turn from Blue to Black. This means the features can not move and everything is now fully defined.
This is important in that you know that everything has been locked down on the sketch and you have not forgotten to dimension any element of the part.
This becomes even more important when using your parts in an assembly.
You would also find that your drawing would shift positions on the page, should you move the sketch defining the part.
Personally I would also define the holes as a separate sketch, only from the point of view that it is easyier to modify later on.
Be careful on how you define the positions of your holes, you need to consider what your design intent is should the design need changing later. i.e. if the postion of the holes are relevant to each other, but not really relevant to the outer profile shape, then dimension that way. If you wanted to change the size of your plate, you will lose the positional relationship between your holes in your case.
Hope this helps.
Cheers
Brian.