Message 1 of 15
I can see VX is great for adding standard parts (bottom up style) but I'm really struggling to get to grips with top down style.
Other systems let you create new distinct parts in an assembly mode, so it is relatively easy to work top down style. Think Design was like VX in that it had a common part/assembly environment, but at any time you could select a shape and say "make component". With VX there seems to be no easy way of doing this apart from copying and pasting parts - which I do, but this seems to unlink references from the part to the original shapes.
This is one area that other more common systems do really well, and it is perhaps the most confusing issue for new VX users who come from other systems. I really do think it would be beneficial for the user manuals to include a tutorial on top down procedures for something like a simple electronics enclosure (or perhaps the mobile phone example already in the manuals could be changed?) to demonstrate best practise and how to maintain history, create a drawing with balloons and BOM.
I know there is a command to insert "empty" parts (insert sub part) but is there a way to convert existing shapes to components without having to go copy paste then redefine the assembly in a new "assembly" file?
BTW I'm posting this here rather than asking my local guru because its probably something that a lot of others might like to know about as well.
Message 2 of 15
Well, VX delivers everything you would expect for Top Down Assembly (which we could do way before many of the other mid-rangers, and some still do not provide essential tools).
OK, VX Part Object Space can be used either for a single body part or a multi-body part or a multi-component assembly. The reason we have such infinite flexibility is because you could easily, say, begin a design as a single body then later find that it requires more than one part to satisfy requirements. In VX, such changes of logic do not matter at all.
From the top then , to build a top-down assembly:
1) Create a new Part Object and give it a name that suggests it is an assembly. When you are in this Object, you can think of it as "Component Assembly Model Space".
2) Right-mouse click in the display window and choose "insert component". Since we are designing from scratch, there is no component object to insert, we are thus creating a new Part Object "on the fly". Give it a name (and optionally select a datum, not normally required for the first object in your assembly of course).
3) Look at the blue VX title bar now. You are actually now in the Part Model Space of your new object. However, you can still see, and select for reference, any other member of the Component Assembly in Component Assembly Model Space. Put it to the test - draw a simple shape, then hit the "Go up to Parent Object" button (6th button from the left on the top-most horizontal toolbar). This takes you back into your Component Assembly, and of course you can still see your first component.
4) Repeat steps 2 & 3 to make another component. Easy eh?! Now, from Component Assembly Space, you can click-through to any component's Part Object Space to work on it - just double click on the component, or select it in the Assembly Manager list. Could not be easier, and if at any time you don't want to see the other members of the Assembly, just hit the "show target" button (top-most horizontal toolbar, 6th button from the right).
Now, if you go to your Root Object List you will see that you have 3 Objects - Your Component Assembly Object and two Part Objects.
It can be best in terms of Assembly MB size to design top-down in this way. To understand this, from the Root Objects List, verify the size of your Assembly Object. Now verify the two Part Objects. The assembly, which "contains" both of the Part Objects as components, is smaller in MB than the Objects themselves!
However, you can define an "assembly" as a collection of Shapes in one Part Object Space. When you have multiple Shapes in one Part Object, you have to be careful that adjacent Shapes do not get booleaned together automatically . Further more, there is nothing logical in a multi-Shape Part Object that is going to tell the auto 2D view layout that the Shapes should be "seen" as being seperate items. With all that said, you CAN build a small assembly like this (technically, this is not a "top down" method, it is a "flat" method of defining an assembly). The good news is that it is possible to enjoy all the advantages of the flat assembly method, then later create a proper Component Assembly based on it.
The VX tool to create a seperate (Root) Part Object from a Shape in your Flat Assembly Object is in the drop-down edit menu: EditCopyGeometry to Part. Once all the Shapes have been turned into seperate Part Objects, you can then insert them as components to make a new Component Assembly. Of course, there are two VX DAL programs in the downloads library that automate this process for you - BatchCreate and MultiComp
Message 3 of 15
I'm sorry to pester like this but its something that every VX new user will face and as far as I can see there are some inconsistencies with the approach VX takes to assemblies.
I've attached a v10.7 assembly file created in the way Chris explained above - so far so good.
This is as simple an example as you can get but it shows some issues (I think).
Part 1 was created in the context of the assembly file. I then anchored this component (as is good practise).
Part 2 was created in the context of the assembly but immediately I noticed an issue.
1. When adding a new "in context" part (right click>insert component>name it>select extrude>middle click to sketch>insert skecth plane) you cannot seem to place the sketch plane on any face of the already inserted component. So, how do you create, say, a part that sits on top of another part's face?
Back to the assembly.
What I did then was create Part 2 on the xy plane, then manually referenced the edges of Part 1. Then toggled the reference edges from reference type to line type.
I then extruded up applying offsets to get a thin walled part.
The next issue:
I went back to Part 1, edited the base sizes and regenerated, Part 1 updates OK but Part 2 doesn't - even though it referenced the edges of Part 1.
The only way to update Part 2 is to manually go into the sketch and regenerate the external references. To me that is not a logical way of working. Surely both parts should update when you hit regenerate in the assembly file?
This is obviously a very very simple example. What about when you have a complex file with several parts?
I'm not knocking VX in any way - thanks to Chris at IDS I have seen many ways of doing assemblies but I still get back to the fundamental issues that if you are moving from other 3D systems to VX, or even a new 3D user, the top down approach in VX is not as clear as it could be.
Perhaps it is simply that the regenerate external references needs to be linked to the main regenerate button - I don't know. But what I'd really like VX to do is have a simple step by step top down assembly tutorial showing how to start with a base part then build other parts using that base part (and new parts) as reference geometry.
In other competing systems you can generate external references between parts from part edges, faces, sketches, points, whatever. Change the referenced part and the whole lot updates. That can be MADE to happen in VX but it does not appear to happen automatically. For an expert user thats OK, but for a hassled designer working on a deadline this is just another source of potential error.
I know in v11 there are interface changes afoot. Perhaps a quick appraisal of assembly methods should be added?
Be interested to hear other user's view on this.
Message 4 of 15
Whoa! I think you need a little more practice . With more time you will see that the VX Assembly methods are pretty good, as is the logic. We have tailored it with the guidance of many customers, some of whom produce very large assemblies. Take a look at http://www.masquito.be/. the entire helicopter, including the engine, all modelled in VX - every last nut, bolt and washer! When things are different to what you are used to, it can sometimes take a while to get the hang of a different approach. This is a quick reply (it's midnight!). Let's go through your points:
1) Anchoring a component is indeed good practise (providing that component does not move at all "in the real world" ).
2) You can place (predefine) a datum for a component anywhere in the Component Assembly Model Space. If you want to relate the datum to the face of an existing component, you can pick the points "on the fly". Select the 3-point datum command and place the cursor over the component face, near a critical point and a preview point is displayed. Alternatively, hold the F7 key down and you can pick any critical point on any component geometry to define reference points (shown as a red triangle symbol). If you do not need to completely control orientation, then you can simply pick a planar face on the existing component "on the fly" when you active the Insert Component command.
3) On Part 2, you say you toggled the reference edges. If that is from Reference Type/Reference Only Type to Plain Line Type, they are no longer reference, and so they will not update with the other object. If toggled from Reference Only Type (dotted font) to Reference Type (continueous font), they will update with the related object - either after an Assembly regen or Individual Part regen, depending on what you have chosen.
4) You can determine when a Part Object should or should not update. When you use Insert Component, check the option "Auto Regen" and the new Object will regen when the Assembly is regened
5) Tutorial: Assembly is covered in the help (and the PDFs on CD), and in the Training Course. That said, you are right, a step-by-step tutorial would be good.
Message 5 of 15
Originally posted by: ChrisW
Whoa! I think you need a little more practice .
Very true Chris. I'm getting there now though, I think!
2) You can place (predefine)?a datum for a component anywhere in the Component Assembly Model Space. If you want to relate the datum to the face of an existing component, you can?pick the points?"on the fly". Select the 3-point datum command and place the cursor over the component face, near a critical point and a preview point is displayed. Alternatively, hold the F7 key down and you can pick any?critical point?on any component geometry?to define reference points (shown as a red triangle symbol). If you do not need to completely control orientation, then you can simply pick a planar face on the existing component "on the fly" when you active the Insert Component command.
My fault that one - I keep forgetting the right click options for selecting points/faces etc. Is there a selection for choosing the centre of a face when doing this? Or ideally being able to select a face and choose a point off the plane to project into the datum plane as an origin? Or do I have to define a datum plane first?
3) On Part 2, you say you toggled the reference edges. If that is?from Reference Type/Reference Only Type?to Plain Line Type, they are no longer reference, and so they will not update with the other object. If toggled from Reference Only Type (dotted font)?to Reference Type (continueous font), they will update with the related object - either after an Assembly regen or Individual Part regen, depending on what you have chosen.
Sorry I didn't make myself clear there. I started the sketch, selected reference curve from edge or silhoette to get the red dotted curves. I then right click and select toggle type to get sketch geometry. To be honest though your auto regen check box tip has sorted that issue out.
4) You can determine when a?Part Object?should or should not update. When you use Insert Component, check the option "Auto Regen" and the new Object will regen when the Assembly is regened
Thats one I missed thanks! I did notice though that if you edit part 1 say, and flip back to assembly mode, the regen button doesn't go green so there is no visual reference that an assembly update is needed because a part in the assembly with referenced edges has changed. In simple stuff this is obvious but a bigger file this might be a problem. If you hit regen anyway everything updates correctly.
5) Tutorial:?Assembly is covered in the help (and the PDFs on CD), and in the Training Course. That said, you are right, a step-by-step tutorial would be good.
My suggestion remains something like a simple electronics enclosure.
Model base parts (PCBs.batteries,etc) then build the skin, buttons etc, create a drawing or two with BOM, then make some changes! Would also be a great demo.
I'm getting there - honest! I'm going to do a screen recording of a simple top down assembly soon, as a thank you and to help newbies get a grip of this fundamental issue.
Message 6 of 15
Apologies if I missed a stage or two out but this method does work pretty well.
Message 7 of 15
Message 8 of 15
I was going to give it 10/10, but you forgot the choc-ice and popcorn........
If an assembly is large, it can be difficult to click-through a component because others are in the way. Not to worry, in this event you can simply pop-up the Assembly Manager and select the component for edit from there. you can also selectively blank/unblank with the Manager.
Message 9 of 15
Message 10 of 15
Message 11 of 15
Message 12 of 15
Message 13 of 15
Message 14 of 15
Message 15 of 15
- autocad 2012 serial number
- how to open dwg on ipad
- cad forum
- autocad 2013 product key
- autocad automatic saving command
- Download free 3d models
- cad for students
- convert dwg to dgn
- how to create fillet in autocad
- DXF converter
- autocad autosave location
- dgn converter
- how to convert text to mtext in autocad
- cad software free download
- mechanical design software free download