Hi there is anyone here familiar with Mastercam?
i want a way to move my origin point just as easily as i am able to do it on mastercam. how is this possible if it is? thanks.
I have no idea how it is done in Mastercam handles it. The only way to do it in SolidWorks, other than going back into the modeling of your part and redoing it with the new origin/orientation in mind, it to use the Move/Copy Bodies command. It's not very hard to do, but does have some drawbacks. (Only the bodies move, so if you show a sketch, it will still be in the "original" position, which can be a bit confusing.)
Adf, moving an origin in SolidWorks is problematic because the purpose of an origin is to provide a benchmark that is stable at multiple assembly levels. A movable origin on a component would have the same effect has there being no origin at all.
I can suggest some ways to situate a model with respect to an origin the way you need it
You can insert the assembly into a blank assembly and mate it to the origin so that you have a positive coordinate reference
You can create a coordinate system in a model file and specify that coordinate system as the origin when you create exports like IGES and STEP
You can open a part file and use "Move/Copy bodies" like Jerry suggested, Just heed his warnings.
you can open the assembly, and re-mate it to the origin.
thanks, guys but do you recommend 3D sketching
or what are your thoughts on 3D sketching because i think it is what i am doing on Mastercam although Mastercam makes things a lot easier.
Well, I don't use 3D sketching for everything. You can't use a 3D sketch as a sweep profile (even if you use 3dsketch on plane) or a revolve sketch or for a wrap feature. Most of the time, it's not practical to use a 3D sketch for an extrude or a sketch pattern. But you definately should know 3Dsketching to make full use of boundary, loft and fill features.
It's also really good for laying out complex top-down assemblies or setting up surfaces.
Do the 3DSketching tutorials and get your head around the basics of using it.
I have worked with both programs for years, and I think you are mistaking SolidWorks design intent for how you would design a work piece MasterCam.......they are two totally different animals from a drawing or sketching stand point, this being said........they do work together fairly well !!!!
You need to stop trying to use Solidworks as if if was just another version of Mastercam. All you are doing is making life hard on yourself. Mastercam is a cutterpath creation system, that has slowly added design/modeling tools over the years. As such, it is a very poor modeling software (but pretty damn good for cutterpath creation). Solidworks is a solid modeling software, that is what it was from day one. (Mastercam Solids is a relatively "new" addition to Mastercam.)
Question for you...
Why do you feel you need to "move" the origin? What are you doing, how are you using it, why do you move it?
Odds are, there is a MUCH better/easier/faster way to do what you need to do...
ok but i don't think i was doing that
i was simply pointing out what i thought was a flaw with SW and giving an analogy that makes sense.
like the other day i was creating this rib and it was frustrating because every time I created a plane (how come you can create a plane whereever you want to put it and can't create an origin point???) the origin point would end up at the bottom.
there are a lot of examples. i just need some flexibility with that origin point. do you comprehend?
Afd, can you post a screen capture of the part you were working on the other day and show us where you wanted to create the origin and for what purpose?
It sounds like there's a disconnect at work here and if we saw your circumstances and understood how you were trying to use Solidworks, we could suggest an alternative approach. I've deisgned a lot of different parts of varying complexity and I can't recall any situations where I thought I was hamstrung by not being able to move the origin.
There is something you need to understand about an origin...there can be only one. It cannot be moved. Things can be moved in relation to it, but it must be fixed. A coordinate system, on the other hand, can be many. One part can have as many planes, axis, & coordinate systems as you desire. In Mastercam, you may think you are moving the "origin"...you really are not (I used Mastercam for many years)...you are simply creating a UCS (user coordinate system) or a reference point, which is not the same thing.
Afd Dfsa wrote: .... there are a lot of examples. i just need some flexibility with that origin point. do you comprehend?
Afd Dfsa wrote:
Post examples here.
I am a former machinist myself (8 yrs on the shop floor).
I think you are confusing part origin with the sketch origin - you can pretty much ignore the sketch origin.
When you make a part out on the shop floor the most robust technique is all dimensions from a single datum origin.
That is the way you should model in SolidWorks.
Based on my years of experience in teaching SolidWorks - I think this is just a matter of logical technique.
I have never needed to move the origin (you could move the part relative to the origin, but that is extra work that is not needed.
I am quite certain there is a easy and entirely logical technque - it would be best to demonstrate on you actual part.
I understand your situation. I use Mastercam as well and the drawing features and ease of movement of entire portions of sketches makes Solidworks frustrating at times. I found an easy solution for my very same issue.
( but like earlier stated it is not as important to your Solidworks drawing as it would be to your Mastercam drawing )
I take the part in Solidworks and save a version as a X_B File (.x_b) this will allow your Mastercam to open the file in a solid model.
Take that solid and set your origin where it needs to be, save it from there as a X_B File (.x_b) and open in Solidworks. prest o - chang o origin moved where you want.
People who use Solidworks and never used Mastercam will not understand the situation you have so hope it helps.
And before anyone thinks that is knocking Solidworks. I am not, it is just a different animal.
hope this helps someone someday, I appreciate the sharing from everyone here. good luck
------ drawbacks are that complicated features may not be recognized by Solidworks once reopened --
WHY when you created it there in the first place it isn't smart enough to see that escapes me???
not fool proof but pretty handy because Mastercam has great tools Solidworks should take some notes on
I ran across your exact situation years ago and found a solution that works very well. I was creating mold designs where some parts required CNC milling, WEDM, SEDM etc. All had multiple setups and origins, depending on the machine in question.
Here's what I recommend - Open your part in SW, and create a coordinate system for each machining operation required. Now, export the part in any flavor that you prefer - IGES, STEP, Parasolid etc. The choice is identical for all export methods, which is this - down toward the bottom of the export window is a box that allows you to choose a coordinate system to use for the export. Select it, click OK and voila !! your part will now open in MC, oriented exactly the way that you plan to machine it.
The beauty in this, is that you can make changes to your SW model, re-export it and it will orient just the same as last time. Very helpful if you already spent a bit of time developing machining strategy, etc.
Let me know if this works out for you. All the best.
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