Z orientation 3

[pejaer]

Hi All,

I want to try to solve what I hope is a basic template "problem" for those of us that use both CAD and CAM packages and do some CNC milling...I am sure this must be already been discussed and solved zillions of time s .

I want my Z orientation in Solidworks to match my CNC mill, i.e. the Z moves up and down and is vertical to the environment, making x-y on the table plane with Y pointed away from me standing in front of the mill, or sitting in front of my computer doing the design work.

I worked with my reseller probably a year ago to re-orient my starting planes in SW to be just this....Z up and down and Y pointing away (see attachment of sketch on RIGHT plane). This was a partial fix, because unfortunately, when working in the right plane, you can see that whereas the view orientation is "correct", SW still thinks it is working sideways....most visibly, the RIGHT plane text and dimensions are sideways. More importantly, any "vertical line" is not vertical, but horizontal, you can see the horizontal relation in the vertical line in the sketch. Also, if I hit the "normal to" view button, the view spins 90 deg, and the relation corrects itself, BUT that is not the environment I want to work in, because Z is not up and down in this case (and gets confusing when setting up the mill and designing for it....). The workaround has been using the Right selection in the orientation pop-up box (lower right) and that at least puts Z back as shown in the attachment.

To get this far, I recall that I ended up deleting the original planes from the tree and creating new base planes somehow using the update or new in the orientation pop-up box....not exactly sure how now.

Am I missing as easy fix?

Thanks
Paul

 

[mjcole]

rollupswx,

My Default Datums are named
X=0
Y=0
Z=0
0,0,0
because that's what their equations are.

Of course Exporting to a Neutral file using a created CSYS would work but if SprutCAM can open SolidWorks.sldprt files directly then that would be unnecessary.

I know many people do not care about this topic because they are so used to XY being the Front orientation as it is on Proe/Creo. However NX and Catia both have the Z axis pointing up off the Top Plane. If Paul used that csys orientation he'd have his default sketch directions messed up because of the way the datum orientations are always set to 1 default sketch H and V direction.

I'm attaching my modified orientation Part for Paul for him to test out. I will probably make an FAQ as well and file a few enhancement requests if the 2013 view cube has the same issues still. I made my Part in sw2010 so most any current SolidWorks user can access it.

imho Paul's VAR just gave him a simple answer and didn't even think of using the "Modify Sketch" tool which most SolidWorks users don't even know about unless they've taken Advanced Part Modeling Class.

"It's not the size of the Forum that matters, It's the Quality of the Posts"

Michael Cole
Boston, MA
CSWP, CSWI, CSWTS
Follow me on !w¡#$%
@ TrajPar - @ mcSldWrx2008
= ProE = SolidWorks

 

[mjcole]

rollupswx,

RE your last comment.
My Default Datums are named
X=0
Y=0
Z=0
0,0,0
because that's what their equations are. I Dislike Spaces in the Tree because the search box is horrible but that's both here and there. Evidently the Righ tHand Rule does not apply to plane orientations.

Of course Exporting to a Neutral file using a created CSYS would work but if SprutCAM can open SolidWorks.sldprt files directly then that would be unnecessary.

I know many people do not care about this topic because they are so used to XY being the Front orientation as it is on Proe/Creo. However NX and Catia both have the Z axis pointing up off the Top Plane. If Paul used that csys orientation he'd have his default sketch directions messed up because of the way the datum orientations are always set to 1 default sketch H and V direction.

I'm attaching my modified orientation Part for Paul for him to test out. I will probably make an FAQ as well and file a few enhancement requests if the 2013 view cube has the same issues still. I made my Part in sw2010 so most any current SolidWorks user can access it.

imho Paul's VAR just gave him a simple answer and didn't even think of using the "Modify Sketch" tool which most SolidWorks users don't even know about unless they've taken Advanced Part Modeling Class.

http://help.solidworks.com/2012/english/solidworks/sldworks/hidd_modify_sketch.htm

Link to 2012 HELP RE: Modify Sketch Tool
Tools > Sketch Tools > Modify Sketch

Image 1: Front X,Y default view's Hz & Vt positive directions

Image 2: Top X,-Z default view's Hz & Vt positive directions

Image 3: Right -Z,Y default's Hz & Vt positive directions

My template with Feature Comments "Xaxis=Right.-Yaxis=Front.Zaxis=Top.prtdot" is attached at the bottom of this post.
# E n g T i p s P o s t , # S o l i d W o r k s

To enable them to be seen use Hide/Show Tree Items in System Options > Feature Manager and set "Annotations" to Show. Normally the Default is set to Automatic which will display them only if they exist. If set to hide they will not show.
This will display existing commments for features when hovering over tree location
There is also a Folder called Comments that lists all the features and comments.
You may RMB Right Click and Select Edit Comments to remove them but I felt it more educational to keep them in part file.

Maybe Paul will be the only this benefits but I'm glad to help out people who like to think outside the orientation dungeon of SolidWorks. To each their own in my opinion Theirs no wrong way to do CAD unless you use Inventor.

"It's not the size of the Forum that matters, It's the Quality of the Posts"

Michael Cole
Boston, MA
CSWP, CSWI, CSWTS
Follow me on !w¡#$%
@ TrajPar - @ mcSldWrx2008
= ProE = SolidWorks

 

[laik]

Hi,
The whole problem lies in the fact that software developers have transferred the classic drawing board to monitor. And the "z" axis is oriented perpendicular on the monitor, as well as the top plane. Apparently they did not realize that it had tilted 90 degrees, so that the axis pointing up. And this in today is not corrected.

 

[pejaer]

Hi Michael,

Thanks a lot for taking these steps to help solve this issue. Perhaps you are right, I get the feeling I am the only one clamoring for this fix . I see it as almost a bug in this world of infinite customization (Solidworks included....takes hours to go through all those options checkboxes!)

I downloaded your part template to give it a try, and basically, I understand that the concept would be to work with your new planes, the ones you marked with a + and ignore the planes with "-". Makes sense, and I can live with that. I still see a problem that after you make your first solid (extrusion) in the new Right Plane + and then use that face to make another, the sketch reverts back to the default...so now you have some planes with horizontal one way and the others opposite. See attached and you can see what I mean.

I might be breaking here...after all this great effort, my best bet might be to wait for the formal requests into Solidworks to get some action to include this option...or switch to UG (Solidedge I suppose is UG?). Joking of course, but...

Paul

 

[mjcole]

Paul,

I look forward to your positive/negative feedback have you posted this issue on other forums or would you like me to do so for you? I tested this out a bit and made a planar surface from a rectangle sketched in correctly oriented right plane+ and noticed that it came up as you mentioned oriented to default Right Orientation. Edit Definition of the Test Orient Plane and test out the orientation when offset from the Front+ or Right+ planes.

The test offset plane I included if tested with the Right+ plane is given the incorrect orientation and text direction of the SW right plane. In ProE the text for the planes is oriented to the display window and always shows correctly oriented and not vertically as off a default face.

The Key Workaround is to keep the first 3 sketches empty except for the point on origin and the Modify Sketch operation.
For any additional sketches you can be duplicate one of the oriented 3 sketches by selecting the original sketch and a new plane then Insert > Derived Sketch.
Derived Sketches for the most part are used to place multiple duplicates of a complex sketch that always match the original. Before modifying the derived sketch features you can Right Click and choose underive sketch

If you create the original YZ sketch on the default right plane and use the Modify Sketch tool to correct the orientation then any Parallel Right facing plane should get the same orientation when using Derive Sketch to copy the parent sketch.

Previous post's mislinked images
Image 1: Front X,Y default view's Hz & Vt positive directions
Image 2: Top X,-Z default view's Hz & Vt positive directions
Image 3: Right -Z,Y default's Hz & Vt positive directions

"It's not the size of the Forum that matters, It's the Quality of the Posts"

Michael Cole
Boston, MA
CSWP, CSWI, CSWTS
Follow me on !w¡#$%
@ TrajPar - @ mcSldWrx2008
= ProE = SolidWorks

 

[Derwood785]

This is great I just did this to my part and assembly templates. The best part is that if you create 3 new planes with the correct orientation that you need, you can go into System Options - Feature Manager and hide the default planes so you don't even see them. It's like you did your own long overdue repair to Solidworks. Thanks