Huston we may have a problem

david_sohlstrom

Scenario- I create a part that is 4' long 1' wide and 1" thick. It has lots of holes and cutouts. Now I want to make a drawing of it that I can load into my CAM program so I need a DXF. 
Well now there does not appear to be a way to create a drawing without a template. Next there is no way to create a custom page size.

Next problem. I exported my test drawing to DXF. It exported fine with one little problem. It named the file with a alpha numeric name that is 72 characters long. I thought well maybe I need to change the tab name so I did and exported again same thing.

Dave

john_mccullough

david_sohlstrom, the Export as DXF/DWG command in the sketch or planar face context menu (Part Studio) is still the best way to create a full 1:1 2D DXF for CAM. 

You are correct that drawing require a template at this time. Scaling the border to greater than actual paper size around large 1:1 views is a good drawings enhancement idea.

For Alpha the Drawings export commands are using the long file names you describe. It is in the plan to be adjusted to match the way we are handling exported file names in Part Studio.  

-John

_Ðave_

@david_sohlstrom You can window pick and delete the border and title block to get a blank template.

@ Onshape We Will need a way to save a template!

jon_mcintyre

@david_sohlstrom, 
John's comment was spot on, that for the purpose you describe, using the "Export as DXF/DWG" command in Part Studio is the best way to go. 

If you do find other reasons to use a custom sheet size or blank template or custom template, and you have access to another system which can create .dwt files (or a .dwg which you then could rename to .dwt), you could make your desired template there, save to .dwt then upload to your Onshape document and it should be available to you when choosing templates for a drawing. 

We do have plans to improve the flexibility of templates and sheet sizes in the future, so we encourage more specific feedback from all users on how you'd like that to work, including functionality and user interface.

_Ðave_

@jon_mcintyre I tried testing this method of creating a template, I created 2 rectangles for a border converted to dxf from mastercam. Then changed the file extension to dwt and imported into my document. When I started a drawing with the template I got a blank template and also my 4 views were in 1st angle projection.

 Obviously I don't know what i'm doing, would you please elaborate on the process to create a drawing template with a little bit more detail.

Thanks
Dave

bobminer

@da_vicki - Here's some new help documentation that will come out in our next update.  Please let me know if you hit any problems creating a custom drawing template following these instructions, as we can fix the instructions.

Custom Drawings Templates

Onshape provides a number of public drawings templates for you to use.  These templates are typical of what most users would need and may be used as-is by many users.

But if you need a custom drawing template, perhaps with your Company name on it, you may do that by following this procedure:

- Sign in to Onshape
- On the documents page, type "Templates" in the Search box and click return.
- In the document list search results, you will see at least 2 documents owned by Onshape containing drawings templates.  For example "Onshape ANSI Drawings Templates" and "Onshape ISO Drawings Templates".  Open the document containing the template you want to customize.
- In the document, right mouse click on the document tab containing the template you want to customize and choose "Download".
- You now have a file named something like "ANSI_A.dwt" on your computer harddrive.
- Edit that file with another editor - AutoCAD, Ares or some other DWG editor - to customize it as you want.  You could add your company logo, alter the titleblock, etc.

Note while editing:
- There are 2 sheets in the dwt file - one for the first sheet of a drawing and a second sheet for continuation sheets in your drawing.  You may need to edit both sheets.
- The template contains many settings that are helpful when creating Onshape drawings, if the settings are still there.  So you'll generally see better behavior if you avoid removing items from the template and instead just modify, add or move items in the template.  For example, it's fine to add additional text and areas to the titleblock.

Continuing after editing the template:
- Once you are done editing the dwt file, save it to your harddisk with the current name or another name and be sure it has the file extension ".dwt" still. Onshape uses the names of tabs when searching for templates.  So if your template has "ANSI" or "ISO" in its tab name, it will be found when the user clicks on the ANSI or ISO filter in the drawing creation dialog.
- Create or open a new document in Onshape.  This document will contain your custom templates.
- Click on the "+" button in the lower left corner of the Onshape UI and choose "Import" and import the dwt file you just saved.  This will create a new template tab in the document.

Once you've done that, the next time you create a drawing, if you click on "My templates" or "Created by me" in the new drawing dialog, you will see that template tab listed and you can choose it as the template for your new drawing.

bobminer

BTW, a significant set of improvements to the look of our standard drawing templates will be in the next update.  So you may want to avoid spending too much time customizing the existing templates, unless you like the way they look now.

jon_mcintyre

@da_vicki
Right now, you get first angle projection if your MEASUREMENT variable is set to Metric, and 3rd angle if it's set to Imperial. 
We plan to have a separate control for angle projection in the future, since MEASUREMENT also controls other things, such as which units you use by default. 

Still, at least your entities should have shown up.  Perhaps there was a units issue, and they got scaled down to a very small size?  That's just a guess.  Let me know if you still have trouble getting them to show up.

_Ðave_

@jon_mcintyre & @bobminer

I tried the instructions.

 I took an existing template imported into my editor. I didn't edit anything, I just exported it out of my editor and created my own template as per instructions. I ended up with my own template which is exact replica of the exsisting template.

 Ok so far so good, my editor (mastercam) can import and export properly.

 I repeated the process but this time I edited the title block by chopping it down to just a few blocks of data to create an simple generic template. This time I ended up with 2 sheets. The created drawing opened on the 2nd sheet that was automatically called layout and was a blank template with 4 views. The 1st sheet was automatically called Model and contained a black background and white template lines and text with very thick lines (strange), When I started a 3rd sheet I got my created template but it was a bit out of scale.

 Apparently there are settings as bobminer stated and therefore must be very cautious of what you are deleting.

I think 1st and 3rt angle is determined by a setting in the  ansi or iso templates not sure yet still experimenting.

Thanks
Dave
 

jon_mcintyre

Dave, please file a bug with a copy of your .dwt, or a link to its uploaded location in a shared document, so I can diagnose what's going on. 

_Ðave_

@jon_mcintyre My dwt ("ANSI_B - Gen-A.dwt is in this https://cad.onshape.com/documents/9ddfcb70616443448bb54267/w/b5c0cb12831c498992f0af0b/e/25da12be549f4e1f9a58af8e shared with Onshape.

Thanks
Dave

_Ðave_

As an update on template editing, I have found that Draftsight which is free will do a good job of editing the drawing templates.

brucebartlett

@jon_mcintyre @bobminer  Is there going to be links to part meta data on the templates any time soon?

I <also> need metric with 3rd Angle projection to meet Australian Standards, so ability to chose projection type a must for me.

jon_mcintyre

@brucebartlett
That functionality has been in our plans for a while, but as of now it's not scheduled for a specific date.  We know it's important to a lot of people so it's fairly high on the priority list. 

However, the kind of links I'm thinking about are ones which would merely display information about the part in the title block. 

Are you talking about a kind of link where the property of 3rd Angle vs 1st Angle would be somehow taken from the part? 
Projection type seems like more of a drawing-only property to me, rather than something which comes from the part. 
I would envision a drawing properties edit command which would let you set drawing-specific properties like units and projection type.  (I know, units isn't drawing-specific, but there are times when you'd want it to differ from the part's units).
After editing those properties on a template or empty drawing, you could save that as a new drawing template to get the combination you want each time.

brucebartlett

@jon_mcintyre Sorry I wasn't clear with my message I don't want a link between the part and projection type, just the properties. Your plans sound great.

andrew_troup

Another attribute which needs to be decoupled from the "metric vs inch" question is the decimal divider.

At present Onshape uses a comma in lieu of a decimal point for metric drawings, which is generally incorrect outside of continental Europe and its offshoots (including South America and South Africa), and is even incorrect in a couple of instances within continental Europe (including Switzerland).

lougallo

@andrew_troup There are plans to make all these options -> settings that can be changed instead of driving them all from the template.