Standard 3 view is backwards??? 1

[shiftersteve]

Occasionally, I find that the standard 3 view inserted into a drawing file is incorrect. The orthagonal projection is backwards of what it should be. I've been having to insert named views one at a time to obtain the correct 3 views. What might I look for to correct this problem?

Also, how can I demand a custom scale for a standard 3 view. I dont see the option box for scale on the 3 view menu like there is on a named view menu.

 

[bluesman0007]

shiftersteve,

I'll address the first question: Look under Tools-System Options-Display/Selection and look at projection type. Is it set at First Angle?

Dennis

SolidWorks 2006 SP4.0
Windows XP Pro, Pentium4 3.00GHz
1.5 GB RAM, Matrox P650
Logitech Marble Mouse, CADMAN

 

[ctopher]

Make sure when you model the part, the front of the part is showing in the front view. Not questioning your modeling, but I have seen this a lot when what a user thinks is the front, isn't.

Chris
Systems Analyst, I.S.
SolidWorks/PDMWorks 05
AutoCAD 06
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[bluesman0007]

shiftersteve,

I'll try the other part of your question. I don't believe there is a way to command it without maybe going through the API. But then I never create the drawing with standard 3-view format. I always bring in the front, scale it to what I want and create the necessary views off that. I don't think I push the envelope too much. I started out designing using a t-square and a pencil. If you created the front view and wanted to change the scale you got a new piece of paper and started over, or thanked God for the invention of the electric eraser.

Dennis

SolidWorks 2006 SP4.0
Windows XP Pro, Pentium4 3.00GHz
1.5 GB RAM, Matrox P650
Logitech Marble Mouse, CADMAN

 

[wgchere]

Make sure when you model the part, the front of the part is showing in the front view. Not questioning your modeling, but I have seen this a lot when what a user thinks is the front, isn't.

Sadly, most of the time what SWx thinks is the front is really the top. For some parallel-universe reason SWx chose to make the z-axis perpendicular to the front plane instead of perpendicular to the top plane. As a result, the top surface has to be modeled as the front surface, because when it goes to CAD/CAM machining the cutter program is oriented with z-axis vertical--the way it is supposed to be. I can't count how many of my models crashed in the machine shop when they tried to translate the axes to make it work with their software. They finally let me know, and now all my models are on their side.

 

[ctopher]

wgchere, I have never run into that problem. Every shop I have worked with can run my parts with front plane as the front, top as the top. I make all parts as the way they will be machined on the table.

Chris
Systems Analyst, I.S.
SolidWorks/PDMWorks 05
AutoCAD 06
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[rfus]

wgchere,

just create a cordinate system and exoprt in that system. I will create my stock, setup other coordinate systems for 3+2 machinging, and create profile and and boudary skethes which are all exportable as IGES and carry into my CAM package. Or just move your part as the last feature.

I somewhat agree that top implies looking down on Z but does it really matter if you know front is z.

RFUS

 

[shiftersteve]

Thanks Dennis, that was the problem with the orthgagonal projection. O

kay, next question, how in the world can I save my drawing preference settings related to text font size, arrowheads, dimension preferences etc within the System Options/Document properties.

I have reset all of the parameters to my liking and saved as a custom sheet format, but every time I open a new drawing with that format, I have to go back in and reset ALL of my preferences. There has to be something I can do to save my drawing preferences. Any ideas? By the way, how much is this costing me?

Steve

 

[BiPolarMoment]

Make a template sheet and save it as such, then just build upon that whenever you create a new drawing--all the document settings will be however you saved the template as.

 

[CorBlimeyLimey]

The Sheet Format is the "template" for what you see ... the sheet border & title block and uses the ".slddrt" extension.

A document template stores all the settings you mention & uses the ".prtdot", ".asmdot" & ".drwdot" extensions.


Helpful SW websites FAQ559-520
How to get answers to your SW questions FAQ559-1091

 

[EEnd]

Out of curosity, in the CAM packages, when you are looking at the front view, with positive x to the right, and pozitive z up, is positive y into or out of the monitor?

Eric

 

[ewh]

Y is into the monitor (use the 3 finger method to figure it out).

 

[rfus]

Make sure you use the 'right' hand.

 

[EEnd]

I was wondering if they were using a right handed coordinate system. It'd be a thorough nightmare if they weren't. Thanks for the info.

Eric

 

[wgchere]

just create a cordinate system and exoprt in that system. I will create my stock, setup other coordinate systems for 3+2 machinging, and create profile and and boudary skethes which are all exportable as IGES and carry into my CAM package. Or just move your part as the last feature.

Wow! Thats a lot more elaborate than our setup. We did the modeling, they did the cutting with no setup from us. The CAM people just used the saved solid model off the network--our software used SWx models directly.

 

[wgchere]

Maybe that was the problem.

(Why doesn't Eng-Tips have an edit function?)

 

[ctopher]

If the models are created correctly, and you have a good CAM software, no extra setup needed. SolidWorks parts will import directly with very little extra work by the machinist.

Chris
Systems Analyst, I.S.
SolidWorks/PDMWorks 05
AutoCAD 06
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[wgchere]

If the models are created correctly

That was my original point. The CAM software often blew up the model trying to get it to have the proper orientation. We were all selecting the Top plane as the top of our part, but that had the x-y-z axes translated 90° from the CAM software (and reality).

 

[ctopher]

The top plane should be the mounting surface of your part (bottom), not the top of your part. It will be the same as the machine's table.

Chris
Systems Analyst, I.S.
SolidWorks/PDMWorks 05
AutoCAD 06
ctopher's home site (updated 06-21-05)
FAQ559-1100
FAQ559-716

 

[wgchere]

The top plane should be the mounting surface of your part (bottom), not the top of your part.

I meant that the top plane was what was parallel to the top (and bottom) of the part. But on our CAM setup the planes were different:
SWx Front plane = Cam Top plane
SWx Top plane = Cam Front plane
SWx Right plane = Cam Right plane

Our machine shop was in-house, so we didn't send the models, or translate them. When the order came through for parts the model was accessed from PDM and imported directly to the CAM software.