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

 

[ArtL]

All I got was garbage. take a snapshot of screen and send as JPEG

 

[ctopher]

To try to make all of your parts match the machine axis may be a headache.
Model your part how you want. Let the CAM programmers orient the Z that seems fit. If there is more than 1 setup, the Z will be a different orientation anyway.

Chris
SolidWorks 11
ctopher's home
SolidWorks Legion

 

[MartinShane]

Our CNC op. gets surly when given a model that isn't oriented with Z as the vertical axis and origin at the "lower left" of whatever block we send him. Since we generally send him .iges or other non .sldprt files I just drop a new Reference Geometry > Coordinate system in the model oriented so to suit him. Then, Save As> .iges/.stp/etc > Options > Output Coordinate System > (New Coord. Sys. Name)

Its not the most elegant method, but keeps our CNC operator somewhat happier without having to make any systemic changes in solidworks that could cause other confusions.

 

[pejaer]

Hi All,

I appreciate the dialogue so far, but in this case, the point is that I am the CAD and the CAM operator, and when I design a part I would like to think in one coordinate system and it can also cause headaches on the CAM programming side. Most times my CNC parts involve just two setups, flipping the Z axis only...also, my CAM has a plug-in to SW that is nice to take advantage of, for part transfer. I just hit the button and the part exports into CAM with the orientation that is in SW....so, it is a pain to re-orient the part especially if I need to go back and change the design....I need to export it again, and it can mess up all the references after I program all the CAM operations, if the coordinate system is all the sudden different....it is a royal pain to reprogram everything. No, by far the best would be the same coordinate system from the get-go.

Attached is a PDF of the work file.

Paul

 

[pejaer]

PDF

 

[smcdesigner12]

I changed my Z orientation in my part and assembly templates 10 years old and still design this way. Open a blank part, press your space bar to see the views, then click on the front view, right click on your screen and set current view as "Top". You will get a message, Do you want to make this change? click yes. This will change your Z orientation. You will need to rename you planes to match. I deleted the word plane when renaming them so I can tell quickly if a new design is not using the new template. New plane names are Top, Front, and Right. I also added 3 main axis's and a coordinate system to the new blank part. Then save the file as a part template on your server or where ever you have current part template. Do the same for your assembly template. (Note: this will mess up your horizontal & vertical relations in sketches)

Phil M
SW2013 SP2.0

 

[pejaer]

Hi Phil M,

Looks like I have some support from you...!

Can you do me a favor and go back to attachment in my original post (there is also a PDF format) and see if your plane looks like mine? I can live with the horizontal and vertical flipped, if I must, probably the more annoying part is when I hit the "normal to" Z-axis is pointing left until I hit "right" in the orientation box, but then my dimensions read sideways ...are you living with these issues also, or have you found a better setup?

Thanks.
Paul

 

[TheTick]

Our CNC op. gets surly when given a model that isn't oriented with Z as the vertical axis and origin at the "lower left" of whatever block we send him.

I won't call that incompetence. Maybe more like a failure to exercise competence. The effect is the same.

 

[MikeHalloran]

I think it's fair to say that Solidworks gets 'surly' when you want to do things in ways other than what was programmed in as 'standard'.



Mike Halloran
Pembroke Pines, FL, USA

 

[smcdesigner12]

Paul,

In options, under document properties, dimensions, linear, (also diameter and radius) click on the center icon under text postion. This will change your text orientation. I hope this helps.


Phil

 

[pejaer]

Hi Phil,

It looks like I have some other option checked that you don't or vice versa. I have all the text position options in the center icon....I even flipped through the options to see the effect, and the others are parallel to the leader, but the center icon, for me anyway, keeps the text 90 deg in my right plane. Any other ideas are appreciated...such a minor "major" annoyance that I would like fixed if I can...

By the way, my base dimension standard is ANSI and I am running SW 2012 SP 4, if this is a difference...
Paul

 

[mjcole]

Paul,

I brought this up to Matt one of the Product Definition guys
in the new Waltham SoldWorks HQs as he gave a demo on 3d drawings. There are two hings you'll want to take a look at to fix your sketch/dimension orientation.
The first of these is the modify sketch tol shown in tge sketch commands which has a circular arrow and +- symbol. This tool is used to modify the H&V direction defaults for sketches which SW always does as follows.
Front H=X, V=Y
Top H=X, V=-Z
Right H=-Z, V=Y

It doesn't matter what you set your default views to the orientations will always be set to thr default Horizontal & Vertical directions I specified.

You may be able to reset the annotation views, but if not you can create new Snnotation views by picking one of the default views and creating a zFront, zRight and zTop view by picking the desired plane and giving an orientation offset of 90 or 180° to get the right orientation. After doing so you can reorient and activate the default \Front, *Righf, snf

"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
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[mjcole]

Continued. Once you create your own or remodify the *Default Ann click and resetotation views, you can right click and change tge dims to the new annotation view.

The modify sketch option may be a better fix because it will change SolidWorks supremely wrong defailt orientations to ones that match your Z up design intent.

When using modify sketch you can enter a deg rotation + or - for your correct x dir horizon. You can flip the defaulf small axis (X) Large axis (Y) dir by right clicking the balls or right click origin ball to rotate 180.

Another way you can create additional rightly oriented sketches is by making derived sketches which will maintain original orientation and then underive them.



This should help you out. zI'll try to send you some example files next week but try followingy suggestions to get a better understanding by yourself.

"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

 

[ctopher]

Paul,
Just curious, which CAM software are you using?

Chris
SolidWorks 13
ctopher's home
SolidWorks Legion

 

[pejaer]

Hi Chris,

I am using Sprutcam, it is a pretty sophisticated (meaning 3 and 4 axis control) software that is "priced right", but it is buggy. Because of the latter, I would not recommend it.

HI Michael,

Thanks a lot for bringing this up to the folks at SW and providing a detailed potential fix...I have played around with the modify sketch and I can get it to spin 90 deg, but I have not had a chance to try to make this a permanent fix by somehow saving this into a template after spinning. It looks like the initial sketch needs to be created, and I am wondering if I can create it, spin, and delete to create a template. I am also curious how subsequent sketches look; for example, if I spin the initial sketch and extrude a profile, then use the face as the sketch plane, I am wondering which orientation it will be....sorry, I did not get to experiment a lot yet, but wanted to express my thanks to you and those trying to help out...


Paul

 

[ctopher]

Thanks Paul.
I have not heard/read of Sprutcam. I will look it up.

Chris
SolidWorks 13
ctopher's home
SolidWorks Legion

 

[mjcole]

Paul,

I'm working on a Detailed How To, to fix the plane orientations for sketches once you've reset your standard orientations. The Easiest way to fix the majority of the problems is when you reset your standard orientations goto the right view and use Alt+Left/Right Arrow to rotate your view by 90deg so the Z axis is facing upwards then select the Right View name and Update Standard Views. If you do this from the Front or Top views the 90 deg offset from SolidWorks defaults will cause the incorrect Horiz & Vert direction issues.

The Annotation Views which display in the Annotations folder in the feature manager and can be set using the Hide show tree items from right clicking inside tree with no items selected or Part Name selected. The fastest method to correct these is to rename the
*Top/*Bottom to *Front/*Back
*Front/*Back to *Top/*Bottom

The *Right/*Left views will still be 90deg off even if you reoriented the Angle of the Views as described previously. You can fix this by Right Clicking the Annotation View and selecting Edit Annotation View Option. After getting into the Edit mode there is a change Horizontal Orientation which gives a 0-360 slider which can be used then hit the Update or Preview Orientation button to preview what the set view orientation gets updated to. Only the Right and Left Views will have to be updated this way.

With the Default SolidWorks setup with Z along the Front Plane directions, the CTRL+7 shortcut the Front Right and Top planes sketch directions are viewed opposite there positive directions. You'll note that this makes the new Front plane face the Backwards Direction. There is still some work to be done on my already updated view part model and I don't want to upload it in the unfinished model.

Feel Free to acces me via the LinkedIn Eng-Tips group which will goto an email I can access without you or I violating violating eng-tip's policies on email address posting email address information.
Cheers.

"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

 

[rollupswx]

Surprised this discussion is still going on.
Just set the z-direction on part as needed in the CAM software.
Lathe, vertical mill, horizontal mill, on tombstone.... .... all relative to operational need.

 

[rollupswx]

oh, and I guess I should mention that I don't let words like Top, Front or Right Side influence how I use X, Y and Z. I just ignore the words.