Message 1 of 12
At first i thought the new way of automatic referencing within a sketch was a genius idea by ZW, and it probably still is.
But when your models get complex, i have found that you are not actually sure what edges you are referencing within a sketch.
With the new automatic referencing, your sketch geometry is automatically snapping to lots of geometry that is very close together, say 0.1mm apart or less.
I know the old referencing options have been re-instated, but i think you need to be able to turn off the new automatic referencing to avoid constraining to wrong geometry, to let you use specific "Selected" reference geometry in the old way.
Within the sketch environment, is there already an option for turning off the new automatic referencing? Maybe it is already available but i cannot find it?
Message 2 of 12
I agree with you, there is some ambiguity at present.
I am not sure how it is done,but currently the external pick seems to dominate over picking within the sketch including existing user inserted references. This needs to be reversed so that local picks have automatic priority.
In the old days, you needed to use F6 or F7 to reference external geometry. This idea has merit as you had control of just where it was coming from.
Now if that was enhanced so that using the function popped up a list of parts you could filter for referencing then you might have a nice solution.
Another idea might be in making a label pop up to identify the component the pick is selecting. At least that way you would know what it was. You still need to be able to filter.
I think these two combined would cover most cases.
Message 3 of 12
I should probably start a new thread but it is sort of linked.....
With the new way of auto referencing within a sketch, when you create 2D geometry, you can snap to external geometry but your lines and arcs end up un-constrained in relation to the external geometry. So you end up having to go back over your geometry adding constraints. This added time compared to say version 2010 therefore a step backwards rather than a progression.
Then to make this situation worse, Even when i create references (within a sketch)to external geometry, and then create new 2D geometry within the sketch, the auto constraining of the 2D geometry is not as good as in 2010. It's frustrating as the right constraints are highlighted at time of pick, but dont actually get added as constraints????, so again i have to go back and manually add constraints.
Having used 2013 for a few jobs now, i still think the referencing and auto constraining of sketches in 2010 is better than 2013, even though the references fall over sometimes. The actual creation of sketches in 2010 for me is faster and certainly more precise.
There is definitely work to be done here.
I cannot understand what was too wrong with the 2010 version (except the fact reference lines fell over sometimes).
Message 4 of 12
When creating 2D geometry within a sketch. The "Focus" option does seem to work. I can focus on a reference line a few mm away yet my smart pick still wants to focus on a line 2 miles away???
Are lines being picked in preference to reference lines?
If this is the case, maybe the preference for the smart pick should consider distance, making reference lines or lines within close proximity a preference over lines miles away.
Or just get the Focus option to work!!!!
Message 5 of 12
Hi Dave, similar experience in top dpwn modeling.
From with in Sketch which is where most our of part referencing takes place it looks like you have made an 'old' fashioned' external reference.
However when the external geometry is changed, the references inside the sketch do NOT update. BUT they still regen - even if it is now not correct and not truly linked. They are frozen to the time they where made and defeat the purpose of making them.
The solutions is to make the reference geometry via assembly referencing BEFORE you start the sketch. This is not a nice way to have to do things but at least you can reference the reference!
All to clumsy for me. The idea of frozen references is almost meaningless. If we want that we just unlink. All references should be dynamic, that is why we use them.
What needs to happen is that full referencing from with Sketching needs to be enabled.
Further the picks definitely need to focus on local entities before picking external entities. Even global 0 is ignored in preference for some obscure edge of point in the background. In the old days a Function key was required ot activate references external to the active part. IMO this is still the right approach as it removes the focus ambiguity and enusres the user knows where the references are coming from.
Show target needs another option - e.g 2 Show targets. The existing one and another that hides the assembly but leaves the part ghosted. This needs to operate from within sketcher as that is the only place it is needed.
Response as to what happens in 2014 is required ASAP.
Message 6 of 12
I'm very glad you have pointed out to me that that the old fashioned references i have been creating are not going to update should the referenced geometry change.
I wasn't aware of this. I have created a lot of geometry last week in this method, now i have a nightmare ahead of me should i need to make design changes - not happy.
The new method of referencing within a sketch just is not good enough on its own. Its just not precise enough and too time consuming to constrain as it doesn't auto constrain very well. In fact, it very hard to add the correct constraints.
I understand your point about referencing in 3D space before re-referencing within the sketch. I remember reading about this on the forum when 2013 was launched. This is the sole reason i didnt upgrade to 2013 at launch.
Without me using 2013 SP on live jobs it seemed to be fixed, so i purchased the upgrade to 2013 and 2014, but having used it in a live job situation, to me, its still not usable. I can see myself reverting back to my trusted 2010 version and yet again waiting for a version that is sorted in the area of sketching which is where most 3D geometry is born.
The sketcher has got to be precise, quick and robust and sorted before any more new sales trimmings are added.
This software as it stands would not be able to be sold in the UK without major backlash to the re-seller.
ZW team, please get the sketcher sorted for 2014 and advise ASAP what the solution is to be. It cannot go on for another few years!!!
Message 7 of 12
Reply 6# sketchevolution
Hi Dave, what seems to work really well is using the assembly reference tools to import the 'associated' geometry you wish to reference.
e.g reference some faces, shapes etc. Make sure the are associated (default is associated anyway)
Now you do not even need to be in assembly mode to reference that geometry as it travels with the part but retains the relationship. This has it's advantages!
And you can use the referenced geometry directly.
I have found it easy to reference a bundle of different geometries into the part whilst in the assembly, then actual do all the design work just in the part. Solves a bundle of visibility issues. However you still have the reference geometry in the way until it is blanked or deleted once finished with.
So whilst it seems a round about way of doing things it is in fact robust.
It does not excuse the current issues with Sketcher referencing in anyway, but the method is worthy of consideration. Don't throw out he baby with the bath water!
For assemblies that are subsequently dynamic, I still do the initial design in a 'static assembly' (where the spatial relationships are constant) and where I do the external geometry referencing from, then I do a constrained 'dynamic assembly' where I test operability interference, etc. It doesn't matter which assembly you edit the parts in, just don't go changing the positions of referenced parts in the 'static assy'.
The reason for the static assembly is that the references need to be stable - if you move things the references will adjust accordingly with results you may not be expecting.
If anyone else has a better solution, I'd be might interested to hear about it. I don't think it makes any difference what software you are using for top down modelling, you will need to follow this procedure IF the assembly is dynamic - parts have ranges of movement.
Cheers - Paul
Message 8 of 12
We find the system in together very problematic
You should always clear and remake and it is also very easy to enter loop
If you are inventing you must exit and re-enter , and believe it bad to manage
We hope that zw3d changes system, with this we will not be able to work
Message 9 of 12
I appreciate the effort you have put in to help me understand an alternative method. At the moment, i dont fully understand the method and it sounds difficult to manage as an alternative for complex 2D sketches, but when i have time, i will read your post again (Slowly) and experiment. And in the mean time, i hope ZW set to work about improving the sketch environment. (referencing / auto snapping & focus / auto constraining) all need sorting.
Almost forgot to mention.......
Another problem with the new auto referencing in the sketch is that the constraints are not visible on screen (I've tried show / hide constraints but this doesn't work). So when you want to modify the 2D geometry in a sketch by changing dimensions or constraints, its impossible, you end up deleting or physically moving the geometry to edit. But this method leads to problems with following history operations failing.
Message 10 of 12
I am only just doing work now with the new assembly referencing so I learning as I go. I can see how if can be of great assistance. IMO it is an improvement in many ways so it gets a tick. It's the missing things that do not get ticks.
I presume you are referring to the constraints and references created when you measure or constrain to external geometry rather than use manual referencing. How to remove the constraints and references that are automatically created but do not show up.
If you do an Regen External Reference you can see the auto references are bracketed. Play them back one at a time then when the ones you want do delete show up, use undo to go back one step then use the Delete Next(Red X) to remove the reference.
It would be much better to be able to do this directly in the sketch off course.
Hope that helps.
Cheers _ Paul
Message 11 of 12
Have been drawing leaf springs in Top down and just barreled along adding face intersection references from the preceding spring. I didn't even think about this previous discussion.
I set all the parts to auto regen at end.
THEN I change a main spring values(top ranking part) and it should all update but it doesn't.
So what I see happening is that the Regen does not actually work from outside of the sketch.
If I edit the part, then the sketch then regen manually it works.
So now I can see why the problem exists.
Well - what else can I say?
Cheers - Paul
Message 12 of 12
It seems to me there one additional control required for it to be fully functional.
As I have mentioned previously, I use one Static assembly model to build parts then a dynamic assembly to test mechanisms and do most of the designing in.
This means the reference is made in the Static. What I have discovered is that if I am editing the Dynamic then the relational position of the reference geometry can shift depending on the where the part is positioned.
What I need to have is the ability to lock the reference geometry relationship to the initial or a particular assembly model where the reference was made.
I would appreciate comments from the ZW team about this. Does 2014 have this capability?
Cheers - Paul
- using cad to work out area of a shape
- autocad 2010 product key
- pdf to dwg
- how to measure area in autocad
- dgn to dwg converter
- .shx file definition
- 3d models of people
- dgn autocad
- drawing software for metal sheet development
- drawing a parabola in autocad
- buy solidworks 2010
- freecad download
- How to draw a house plan in autocad?
- how to open dwg on iphone
- free cad software