How to change cylinder diameter in ST? 1

[mclaser]

It's got to be simple but can anyone tell me how to change a cylinder's dia in ST? 1) make a circle, ESC, 2) extrude to cylinder. Length change is no problem with wheel, but what the heck do you click on/select to mod the diameter? I know you can add a PMI dimension and change it there, but that does seem to fly with a more complex model.

Greg

 

[beachcomber]

Haven't seen it yet but suggest click the cylinder, then RMB. Anything on there for resize ?

bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.

 

[donyoung]

Greg,

for a cutout it's the way to go. For the sketch is
no longer used as soon as the feature is created
you now have to shift most if not all dimensioning
into 3D.
Using the hole feature to create the hole then you
can place the steering wheel on the hole and select
the dimension

@BC
that will no longer work

dy

 

[mclaser]

Thanks for the input. After playing around a little more it looks like you can use dims for modifying reasonably simple cylinders, but tapers (including drafted cylinders) and curve revolves are another story. You can move the flat ends with the wheel but it doesn't appear as though you can manipulate the end or side profiles. The wheel will attach to a quadrant point on the end profile, but the circle will only move as a whole entity. I've included a pic of what I'm doing if anyone wants to try to replicate and see what they can come up with. Also, anyone can figure how to change the radius of the groove on the cylinder, that would be great!

Greg

 

[donyoung]

Hi,

for the rotary cutout (groove):

use 'SmartDimension' or use 'Distance between'. Set keypoint type
to 'Center Points Only' and select both edges of the coutout.

Now you should be able the change the radius of the cutout
through the dimension. Using the wheel will only move the
cutout.

dy

 

[mclaser]

Thanks dy. Yup, that works. Still can't figure out how to change curve sweeps or the end of a taper (ellipse). The wheel will snap to a quad point but it won't change the shape of the profile. Best I can do is either add or remove mat'l with another sweep/revolve.

Greg

 

[donyoung]

Greg,

yes. I think the only way to change the shape of the other
items is to remove/add material. After the creation of
a feature it's just a collection of faces and nothing more.
So one can't neither change nor delete some 'features' after
creation -- no 'healing' of the faces is possible.
OTH: a hole created through cutout can be dimensioned to
change the diameter. A true hole still knows all it's
data depth, thread, ... But a draft does not remember
the angle -- I think there is some room for improvement.

FYI: open a draft to do just some sketches (2D only) you
will notice that to dimenension the sketch one has to switch back
to 'Home' to do that. This is accepted as bug it will be
fixed with the next version (language dependency prevents
fixing it by a patch, because a patch is language independent)

dy

 

[donyoung]

Greg,

to remove a draft from the model you can do this:

select Draft function from the menue
make sure Face is selected in the pulldown
select the bottom plane/face (the original base plane for the draft)
select all the draft faces (only these!)
set the angle to 0 and press enter

Now a new draft is created at angle 0 which whipes out the old one
which is still shown in the feature collection

dy

 

[mclaser]

Thanks Don. Nice tip! I guess I never thought about using the draft function to de-draft a draft! At that point it looks like you're stuck with the draft as it's apparently intimately connected to the protrusion. Oh well.

ST is almost starting to get me a little excited, until I get spanked down by something that used to be simple to do. This version is unfortunately very frustrating thus far (~5days).

Greg

 

[donyoung]

Greg,

to use the ST (sync) modus effectivly you have to forget
most if not all what you know about modelling the traditional
way ...
Create a rough sketch, no need to constrain, extrude it and
then put it to shape. Remember the sketch has no conection
to the feature once it is cerated ...

The tip to set the draft to 0 deg was posted in the UGS NG
I've tested it and it did work so I passed it on.

To get rid of a draft you may also try to select the drafted face
and the use the Relate option with Perpenticular and Persistent
option selected. As target plane choose one of the two other
planes that make up the draft's angle, and do an RMB (= accept).
The Pathfinder should show a topic'Relationships'.
There is, however a bug in that the relation will not be
honoured immediately you have to move one of the planes that
is adjacent to the plane that has been chosen as target plane
(or just the target plane)

dy

 

[donyoung]

/Edit

the first remark about sketching in ST-mode relates to
simple geometric forms for others it might be neccessary
to have the sketch accurat. To bring them to shape later
on is either impossible or difficult

dy

 

[teebarr]

Greg
This new version has been tough. In trad. mode I can't find anything with the new interface. Switch to ST mode and as dy says, it genuinely is a total change of approach. It is a new modeller - not just SE with add-ons.
As I start to get used to ST I can see the depth the development team have gone to in order to deliver a well thought out revolutionary modeller. For a V1 it is impressive. Sure there are some things not quite there but I understand many of the obvious ones will be fixed for V2.
I am now getting to get to the point that working in trad. mode is starting to feel cumbersome. My guess is soon I will not go back.
Looking forward to sheetmetal in V2.

Tony

 

[beachcomber]

Hi All,
I've been watching this thread with interest as my colleague has just gone on a 2-day ST course (only permies get to go, not contractors)
I get the impression that ST is good, but there are still some things missing (Sheet Metal?).
Can anyone give me a brief of what is missing or what doesn't quite work yet? What about XpressRoute, Surfacing etc? Can you delete features and do re-ordering?
The other thing is, ST is not V21 but will there be a V21 of the 'traditional' type.
I'm still not convinced about the direct modelling approach.
I can see benefits but if I go to the trouble to draw a fully constrained feature profile or sketch I don't relly want to lose it when the feature is created.

bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.

 

[donyoung]

just a short info: ST is actually a hybrid CAD as you can
work in synchronous mode or in traditional mode.
You can see the trad. mode as V21 it has all functionality
the V20 has -- the GUI, however is that of Office 2007.
The new mode is the ST mode which lacks
- Sheetmetal
- Insert Part copy
- FOA, FOP
....

Draft is the same for both modes.
By selecting the appropriate template you will be either
in traditional or synchronous mode. You can not switch
dynamically between these modes. A traditional part can
be converted to a sync. part but this is 'one way'.
Both assemblies (sync or trad.) can hold parts of both
environments.

dy

 

[Raaden]

ST is also missing assembly features and the ability to make threads.

Btw, what does FOA & FOP stand for?

 

[donyoung]

FOA = Family Of Assemblies
FOP = Family Of Parts

dy

 

[teebarr]

bc
Sheetmetal will come with the next release Q2 2009.

"Can you delete features and do re-ordering?"

You can delete features if it can heal, otherwise - no. Re-ordering is not possible - as there is no order for re-gen. ST is all about faces not features, so the "tree" is really just a handy way of selecting faces as opposed to being editable features as previously known. You no longer select features that you can go back into and edit, once they are created you edit them directly. This is the hardest bit to get used to and is where you need to understand the face selection tools and live rules. I think this has been the steepest learning curve.

Alot of the techniques you use today are no longer valid. However, fully constrained sketches are - sort of. The sketch is no longer used (but can be accessed for re-use) but the constraints that were applied to it transfer to the faces that the sketch created. So fully constraining geometry is still possible.

ST patterns are easy to use and work well for certain situations but there are currently some shortcomings. There is no way (that I know of) to dimension the occurance box to a face, you are only able to specify the box size. Also, large patterns are very slow - unuseably slow.
As I said before, this is V1 of ST and as such is very impressive indeed. However I think it will take some time before trad. mode is no longer required.

Tony

 

[donyoung]

Hi,

[...]
You can delete features if it can heal, otherwise - no. Re-ordering is not
possible - as there is no order for re-gen.
[...]

this reveals one difficulty now: ST -- but which mode? The new version is
called ST (internally it's V100). So the above is valid for ST, aka.
synchronous technology. Talking of traditional mode (V21) you can delete them
as usual.
So when the new version is out everywhere and asking for help IMHO it's
neccessary to specify the mode whether it's V21 (traditional or TE) or
ST (synchronous)

dy

 

[mclaser]

I think you can add to list of excluded functions in ST that there's no Divide Part and you can't really edit a surface outline created by a curve sketch (ie. revolve, sweep, etc.). Dan mentioned on the UGS forum that this is coming. I have, however, been able to edit a model created by a curve profile, but only the section that has a defined radius. Clicking on that surface brings up a "R" dimension which one can change and the faces with re-bind, which is nice.

The big problem with all of these limitations to ST is that they seem to intentionally be kept from the users. Shouldn't there be a comprehensive list provided by the manufacturer so people trying to be productive with their product can make an intelligent choice? Why do we have to patch the evidence together to solve the mystery?

Greg

 

[beachcomber]

Hi everyone,
Thank you for the most enlightening replies.
I suppose I was being optomistic with the functionality of this first version - it's obviously going to take time to get everything into it. Even so there seem to be a few fundamentals missing - and as Greg says, the limitations should be made clear from the start. The impression given by all the demo's is that it is a fully functioning version that would take over from the previous ones.


bc.
2.4GHz Core2 Quad, 4GB RAM,
Quadro FX4600.