You will have to make the portrait sheet format and load that to the drawing. There isn't a "make this portrait" button... or you can just tilt your head sideways ... sorry, couldn't resist.
No, it can't. You will need to change your sheet template.
One thing that Paul and Glenn have not mentioned is that swapping the sheet format is extremely easy (takes about 5 seconds).
On top of all why you need to do that. Are you looking to rotate the views also or just the sheet format?
Looks like you're trying to make a new template? If not then why not make a new template for portrait orientation.
All that I am trying to do is have the view of the sheet to be shown in portriat. We do this all the time in Autocad by just rotating our templates. I would create a portriat of the one I use in landscape but time is the issue. Is there a quick way to take my landscape template and turn it into a portriat?
you can still do the same thing, it probably won't be as easy as Autocad (depending on how exactly your current sheet format is done) but you can still select all and rotate 90°... just probably will take a little bit of cleanup. Can you post your current template?
Martin, I've got a pretty good understanding of AutoCAD. When you say you rotate your template, what steps do you take?
I ask because I'm going to try to advise you in such a way that the resultant Solidworks template is similar to your AutoCAD Template.
So, are you opening the template, using the rotate command to re-orient your border or are you twisting the view. Are you doing this from paperspace or model space? If paperspace, how are you handling the orientations of the individual viewports?
-or are you doing this through pagesetup manager and the plot dialog?
When in Autocad I do an insert find the template I want to use select and accept. I am doing this all in model space in Autocad. The template is now in my model space file as a block. I select rotate or keyin, select the entities by window crossing pick the lower left corner of the template and keyin 90. Template is now in a portriat viewing. Hope this helps.
OK, you threw me there wit your use of the word template.
What you're doing is inserting a drawing as a block and rotating it as opposed to creating a plot configuration and setting the orientation to portrait.
You can do the same thing in Solidworks. As a matter of fact you can do the same thing using an AutoCAD drawing if you want.
Assuming you already have a drawing with a border that you want to rotate, here's what you do:
- Right-click over the drawing sheet area and select Properties
- In the Sheet Properties dialog box, you want to check the 'Custom Sheet Size' checkbox and fill in the dimensions for your sheet size. At this time, make sure you're projection radio button is set to Third Angle (unless you're doing drawings to ISO standard). click OK to exit your dialog. You'll be back in your sheet view. If you zoom out a little bit, you'll see the drawing sheet in the proportions you wanted. The titleblock and border will probably be crossing through it. That's what we'll fix next.
- Right-click over the sheet and select, 'Edit Sheet Format' You're drawing will change to the Sheet format editing mode and you'll be able to see all of your border entities. Now you'll rotate them with a tool that's very much like AutoCAD's Rotate tool.
- Window select the entities and then WITH YOUR CURSOR OVER A SKETCH SEGMENT IN YOUR SELECTION right-click and select 'Rotate Entities'
- Property manager will display the roate interface. Highlight the 'center of rotation' control and pick a point in the field of your drawing. Come back to the rotate dialog and selec the rotation angle control and type in 90 or 270 or whatever angle you want.
- The graphics will rotate. You have to go back to the dialog box and hit OK in order for it to finish. This takes some getting used to so go slowly the first couple of times.
- There's also a move tool that works on a similar principle that you can use to relocate your border graphics back onto your sheet. Window select your border graphics, right-click with your cursor over an entitiy and select 'Move Entities' you pick in the 'StartPoint' control and then select your base point and second point in the field of drawing.
If you are starting from a blank drawing and have a border in AutoCAD, then between steps 3 and 4 insert the following:
This will pull up the insert block dialog. Change the file type from SLDBLK to DWG or DXF depending on your existing 'template' format.
Navigate to your drawing border folder and select it to return to Solidworks. It will take Solidworks a few seconds to load the block graphics but when it's ready youi'll see your border floating around on your cursor just like it does in AutoCAD. Place the block insert on the sheet.
The property manager will have controls where you can set the scale and rotation angle. you can call up this panel at any time by clicking on the block insert. You'll notice there's also a button labelled 'Attributes'. If you click this, you'll get a dialog that resembled DDATTE.
you can explode the block by right-clicking on it and selecting 'Explode block' You can also edit the block in place, save it to a file and delete it from the context menu. Block defnitions are stored in the drawing in the Blocks folder just underneath the Drawing title in the sheet manager. If you want to insert another instance of the border block, you can expand that folder, right-click on the block name and select 'Insert Block'
That ought to get you to where you wanted to go.
However, I don't think anyone works this way in Solidworks. Certainly not with drawing borders and titleblocks. Amoung other things, you can't rotate tables or dimension text (not so that it's all reading at the same angle as your border anyway) and it's a royal pain to type notes sideways. If you have a border that's already been laid out in portrait fasion, you can use that just by changing the sheet size like I talked about in step 2. Otherwise, most of us let the printer driver or PDF writer rotate the border for us.
Hope it helps.