Origin point 2

[ctopher]

I have had several users ask me how to move the origin point. I always tell them you can't, just create the part with the origin on the bottom/center. But I'm curious, is there a way to move the origin in a part/assy or has someone come up with a macro to do this? We are using SW03.
thank you
ctopher
Sr.Mech.Designer

 

[SBaugh]

The origin cannot be moved in a part. You can place a part in an assemlby, and then you have the origin of that part. Then you can move that part around the assembly origin, but that origin isn't moveable either.

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
When in doubt, always check the help

 

[meintsi]

After the completed part has been modeled, you options for moving its origin are reduced but not impossible.

If you need (or want) the origin of the part to be in a different location, it can only be moved via changing the relationship of the initial sketch or sketches (in the case of a loft or sweep) and possibly the feature (in the case of a boss-extrude) to the part origin.

I.E.
Insted of placing the origin on the edge or corner of the initial skecth, place the sketch around the origin and dimension to it or place it away from the origin.

Also , as in a cut extrude, extruding MidPlane or offset will place the origin accordingly.

But these things should normally be thought out before the initial modeling begins.



Remember...
"If you don't use your head,
your going to have to use your feet."

 

[ctopher]

Thanks. We do create our sketches around the origin...the origin in the middle of parts/assy's. It was just a curiousity if it was possible if someone made a mistake and created the part with the origin at the corner, if it can be just moved to the center. Maybe a future version?

 

[SBaugh]

If you change the location of the sketch around the origin, doesn't mean that you moved the origin, it only means you moved the position of the sketch.

You can setup a new type of origin by going to Insert\Reference Geometry\Coordinate System pick the vertex or your X, Y, Z and click OK to make a new coordinate Origin.

The Origin that comes in the parts and assemblies can physically not be moved. only the sketches around it can be moved and adjusted.

Regards,


Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
When in doubt, always check the help

 

[djw2k3]

Just to further this question,

I have created empty drawing views (in a drawing) and placed sketches in them that i would like to custom align.

The "align by centre" etc command gives me some kind of random alignment (haven't quite figured what drives this alignment:-D)

 

[djw2k3]

ops, forgot to add sw 2001+ ;-)

 

[TheTick]

You can use the 2D to 3D tools to move sketches around even if they didn't originate from a 2D import.

All this machinery making modern music can still be open-hearted.

 

[SnowCrash]

I often export part files and need to redefine the origin. I define the new origin with a new coordinate system and export an iges or parasolids file using the new coordinate center as the origin. Of course you will lose the features when you do this.
You might have some success doing as suggested by redefining the sketch planes to new ones based on the new coordinate system. This will not move the origin but it will move your geometry.
Crashj 'and it moves still' Johnson

 

[ctopher]

Thanks. I had a part once that was imported from a company we bought. The part was so complicated and the origin was not near the geometry. When I tried to move the sketch to center around the origin, the whole part turned red. By the time I fixed it, I could have just redrawn it from scratch. It would be nice if SW had a icon that would auto move the origin and auto update the sketch relation. (Just dream'n)

 

[SBaugh]

What you need to do is set up a Coordinate Origin like I & Snowcrash listed above - You can setup a new type of origin by going to Insert\Reference Geometry\Coordinate System pick the vertex or your X, Y, Z and click OK to make a new coordinate Origin.

Then Export that file out as a Parasolid before you save the file click on Options and under origins click the down arrow and click on the Coordinate origin you just made. Then save it. Open the newly save Parasolid. There you should see you part pop back to the origin that you just created.

Regards,

Scott Baugh, CSWP
3DVision Technologies

http://www.3dvisiontech.com

http://www.scottjbaugh.com

faq731-376
When in doubt, always check the help

 

[macPT]

I think you should not neglect the origin position. I allways try to build my sketches so the origin can be at a very well known position (in the center of the part, in the middle of an edge,...).

It's an easy way to easely understand the mass properties data.

Regards

 

[JNR]

hmmm.... OK, here goes. The origin of the universe can not be moved. Mathematical space is there before you start modelling. So the mountain has to come to the prophet as it were. (Apologies to our Isamic friends - I forgot how to spell His name - I'm embarassed.) You will have to move the part geometry to the origin. There are a bunch of methods which are quick/slow/keep/loose data etc. depending on your needs. You will have to choose for exsiting parts. For new ones, start out in the right place.

3/4 of all the Spam produced goes to Hawaii - shame that's not true of SPAM also.......

 

[ctopher]

Thanks Scott. Very good idea.
As I wrote, we always create our parts with the origin in the center. There is those times when we get a part from an outside source that the origin is elsewhere, but to move the sketch so that the origin is in the center is a headache...everything turns red and is a great undertaking to fix it! Better off re-creating it! We had hoped there was a way to tell SW to move the origin to the center and all sketches were auto updated. But we can get around it. Scott's idea works.

 

[TheTick]

When I was working on Pro/E, I would set up my base datum planes on a user-defined coordinate system that could be transformed to any position. If I moved the working CSYS, the base planes and all associated geometry would move with it, and I could move the entire model to any position w.r.t. the absolute CSYS.

Unfortunately, this doesn't carry over to SW for 2 reasons:
1.) In SW, a CSYS can't be used to define a plane. I suppose it would be possible to substitute a 3D sketch, though.
2.) Unlike Pro/E, SW does not give the user absolute control over which side of a datum plane is the front and which is the back. This can wreak havoc with sketch orientations if a plane decides to flip-flop front and back sides when it is moved.

If the ladies don't find you handsome, they should at least find you handy.

 

[MrPickles]

TheTick,

Unfortunate but true about Pro/E. SolidWorks stinks. Long live Pro/E...

Opps, wrong forum....

I shall belittle myself for the rest of the day,


-----------
Mr. Pickles

 

[RawheadRex]

"Unlike Pro/E, SW does not give the user absolute control over which side of a datum plane is the front and which is the back. This can wreak havoc with sketch orientations if a plane decides to flip-flop front and back sides when it is moved."

I am sometimes capable of not being able to recall the ability to select which side of the plane that I wanted past items onto in ProE. <sigh> But when I can't forget (like when I try to copy and paste sketches for instance) I have to get professional help in order to get out of bed in the morning sometimes.

As far as the dealing with the origin point not being in a logical location, well that just plain sucks because the only expeditious recourse that I've found is redfining sketch relations (tedious) or recreating the entire sketch (and correct any errors such a course of action results in).

I suppose it would be nice to move the origin at times but can kind of understand from a programmer's point of view why this probably can't be done. I'm not sure if it has to do with the Parasolid engine or if it's a mathematical thing within in the code itself but I think that's what it comes down to though.



Chris Gervais
Sr. Mechanical Designer
Lytron Corp.

 

[JNR]

Here is a simple method we have apparently used (so I am told - I have not personally tried it). (Mostly on imported aircraft structure models from customers.)

Open a blank assembly and insert the part (or use your existing one if you have one and are confident). Insert a new subassembly (using assembly-new) and mate or fix it's origin where you want the origin of the part relocated to. In the feature tree, drag the part file into the new subassembly. Open this new subassembly and save it as a part file. (You must have SW2003 or later.)

The drag does not move the part in space but only changes the assembly hierachy. When you save the subassembly as a part file it retains its own origin, thus keeping your part data uncorrupted but with it's origin relocated.

The Parasolid method works, but you loose all your features, etc.

3/4 of all the Spam produced goes to Hawaii - shame that's not true of SPAM also.......

 

[ctopher]

thanks JNR. Good tip!
ctopher

 

[Arlin]

> Open this new subassembly and save it as a part file

With this method, you also loose all feature data and associativity. It becomes a dumb solid just as with the parasolid export method.