Copy Geometry in SW

[nawaz]

Hi All,


What is the equivaqlent of copy geometry (available in Pro/E) in SW? pls let me know.


Thanks in advance.


NAWAZ S K

 

[nawaz]

Hey guys,


pls let me know the answer for above query. some body must be knowing abt this...

 

[ralexy]

I was looking for this functionality long time but I found nothing. I use reference directly in assembly. I know it's not good but I think there is only this way.
Example: [url]http://www.alra.ic.cz/_pres/_default/Dir/Silowaggon/Silowagg on_07.gif[/url]
Edited by: ralexy

 

[ProE_Addict]

Nawaz & Ralexy,


Makes you wish you were using ProE, huh? Me too. It depends on which version you are using. Pre 2008 has nothing, but we have found a "work around". We use afeature called "Join" along with assembly references to do something similar (see basic steps below).The method used to relate parts top-down is the "base part". This is extremely limited pre 2008 as you can only bring through planes, axes, surfaces or cosmetic threads(??) along with the entire solid from the part being referenced. 2008 adds a lot of features to what you can bring along.

1. 
   <LI>Create a "base part" from which you want to use references. This should not be a part which is used for anthing other than reference. Look up "base part" in SW help for reference. This part should contain all required geometry, planes and sketches you might need.</LI>
   <LI>Create an assembly and add the base part as the first component.</LI>
   <LI>Turn off the components visibility in related BOMs and change the part weight to zero to avoid erroneous mass properties for your assembly.</LI>
   <LI>Create a new part and add it to the assembly in the default position.</LI>
   <LI>Edit the part and insert a "join" in the part using the solid geometry from the base part. This brings through the solid only.</LI>
   <LI>Show anysketch in the base part you need to use in the new part.</LI>
   <LI>Edit the new part again and insert a sketch on a plane parallel to that which the base part sketch is on and generate a sketch using edges in the new part. This creates a link to the base part.</LI>
   <LI>Lock and unlock the external reference to avoid adding features you don't want in the new part.</LI>
   <LI>Hide the base part in the assembly when you're done.</LI>
   <LI>EXTREME DOWNSIDE HERE--- You absolutely need to be aware of specific sub assemblies you need before you do the above operation (if you don't know, you can create sub-assemblies in SW by selecting several components in an assembly, right-clicking ans selecting "form new sub-assembly here"). If you create your parts related to the base parts before forming sub-assemblies, the parts can't find the reference to the base part once you create the new assembly.</LI>

 

[swcalvert]

Nawaz, what are you trying to copy? If it's a sketch, just select the sketch and ctrl C and ctrl V (paste) it to a new face/plane. If it's actual geometry, then we might need to know more about what version you're running.


Steve

 

[nawaz]

Hi ProE_Addict,


thanks for the reply n info u had provided. i m using SW2007. hope SW2008 has direct functionality for copy geometry. Though initial learning curve for Pro/E is steep, but pro/E is far more powerful than SW in the matter of design control thru' copy geometry n top-down design. i can control my design very easily thru' Pro/Program once i m done with the design. is there any thing similar to Pro/Program in SW? Pls let me know.


Once again thanks a lot for ur info.





Hi Steve,


Thanks for ur reply. I want to copy actual geometry (like planes, axes, points etc), no solids, no surfaces. as i said i m using SW2007. pls throw some light on this. what abt SW2008. is this copy geometry functionality available in Pro/E. Pls note that i m neither criticizing nor promoting any software. ultimate intention is to decide which one suits our needs. v have been using pro/E wf3 (1 seat)for 2 yrs n management decided to increase no. of seats n they are finding it expensive though they r happy with pro/E. hope u can throw some light on this.


Thanks a lot.





-NAWAZ S K

 

[nawaz]

hi Steve,


pls correct my earlier post, is this copy geometry functionality available in Pro/E. to is this copy geometry functionality available in SW2008.


thanks once again.


-NAWAZ S K

 

[ridein]

nawaz,
Since this is a SolidWorks forum, in general we, SWX users, don't typically know or understand ProE commands. So your "copy geometry" 2008 question about ProE isn't something we can easily answer. Where I work, we just got the 2008 DVD's last week.
Please correct me if I'm wrong, but I thought the ProE Wildfire was comparable in price to SolidWorks so I don't see why you would go to SolidWorks if your people understand ProE already.

 

[ProE_Addict]

I've thought there should be an area for CAD users who need to start on a new software to post questions like this...


I've used ProE for about 12 years and work for a design firm. We've been using SolidWorks almost exclusively for the last2.5 years. The top-down design issues Nawaz speaks of is one of my hot buttons. I have several others as well howeverv2007 improved significantly over 2006. I used to have a screen shot from SW of the available features you can bring along with a base part, but looks like I deleted it...


Aside from the copy geometry issue, thebiggest problem we've noticed lately is terrible performance with large assemblies. Nawaz, if you build anything over about 300 components I would urge you to wait on SW. We have 2.33Ghz laptops with4GB RAM and are using the 3Gb switch in windows and SW still takes all the avialable memory and dumps a lot.


I have a list of issues I've noted if you would like to see what I've found.

 

[nawaz]

hi proeaddict, and all,


thanks 4 replies. surely proeaddict pls send me the issues u hav got. it may help me to understand both softwares in better way.


my e-mail id is skareemnawaz@yahoo.com





this price issue i really dont know. let me find out.

 

[design-engine]

"insert part"


the options are similar to copy geometry but you take everything. In Soldiworks you don't get much of a choice like the more mature proe offers but it works basically the same. It is a trick to get the insert part to line up to the default coordinate system.

Try it I can answer most of the questions related to top down design in solidworks even tho we have not officially started teaching solidworks yet.

 

[mjcole_ptc]

Try using the Assembly Layout tools and Named Blocks.

Beginning of Assembly
<a href="http://picasaweb.google.com/michael.j.cole/SolidWorks/photo#5130289032815254242" target="_blank">
Create Block from Layout</a>
<a href="http://picasaweb.google.com/michael.j.cole/SolidWorks/photo#5130289037110221554" target="_blank">
Image 3 Block Types</a>

Image 4 Part From Block
<a href="http://picasaweb.google.com/michael.j.cole/SolidWorks/photo#5130289037110221586" target="_blank">
Image 5 Asm of two block type parts</a>

Layout tools do not allow surface references or 3d entities but you can create multiple blocks and insert them in a single part to create eometry referencing layout sketches on different planes. You can also use the Triad to move blocks to desired positions of geometry and get similar results to Pro/E.

Michael

 

[ProE_Addict]

Design-engine


We thought using "insert part" would do the trick, but it lacks severely in whatfeatures you can reference (this has changed in 2008 and looks like it will be the method to use). If you are used to using Copy Geometry, you are likely wanting to get curves to drive other parts. With "insert part" you have to take the solid as well. I've outline generally what we do in a posting earlier in this topic if you're interested. I can also provide a more detailed version if you'd like.


On positioning the "insert part", if you browse for the part you want to reference and then click the ok button, the part snaps to the "default" position. Aligning origins by drag-and-drop doesn't work well.


Mjcole_ptc:


If you use blocks, are they parametric back to the reference part/assembly?