| Author |
Message |
Diemaker
Guest
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 Posted:
Wed Nov 30, 2005 9:10 am Post subject:
Should I buy SOLIDWORKS? |
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Should I buy SOLIDWORKS?
Long time user of acad, bought Inventor 4 years ago. It's improving
but so has SW it seems. And in my trade SW is becoming the norm... if
you can call a handful of 3d die designers the norm. But the top three
reasons SW is attractive is part configs, individual form control of
sheet metal, and edrawings. Very excited to see if configs can live up
to expectations. So I'm thinking about using my end of year money to
buy SW and have some questions. Oh, I'm foolish for not getting a 30
day trial, but too late now.
1 - I've been using master-sketching to control blocks that nest
against each other. If I understand correctly, in SW, sketch 4
squares,...2 butting, 2 gapped... extrude with one extrude. Then use
split feature to create 4 configs or 4 separate part numbers. Then
there is one file with 4 parts can be a sub in the assy. This would
effectively create a mastersketch, parts and sub within one file??? To
good to be true.
2 - Edrawings. I've only seen relatively small Edrawings. How is
performance with larger models, 200 unique parts, 500 total. Is it real
choppy? Can it be measured, sliced? How big would that file be, approx.
3 - Drawing side views. Dies are basically two halves, top and bottom.
It is common to show the bottom plan view with section lines to the
side views. Side views are a section of both top and bottom. In IV this
is possible with design views, plan view of "both halves" view is
section cut, then "both halves" plan view is replaced with
"bottom only" view, yet the side view still shows "both halves"
view. Does SW have an equivalent?
example: http://img507.imageshack.us/img507/2831/sideview5iv.jpg
4 - Importing a .dwg to the sketcher... can you turn layers on/off?
Widow select entities? Maybe even copy paste a dwg in a sketch? Or do
you have to import a whole file?
5 - Is there window selection in sketch environment? in model? In
drawing ?
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Sporkman
Guest
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| Posted:
Wed Nov 30, 2005 9:10 am Post subject:
Re: Should I buy SOLIDWORKS? |
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Diemaker, I can't say I understand your first question -- maybe someone
else will answer. But for the 2nd thru 5th questions, here are my
thoughts:
2) Performance is generally pretty good on machines which have some
power. Sending an eDrawing of a large assembly to someone with a
typical laptop/notebook computer is likely to result in some frustration
for the recipient. Size of the eDrawing can vary greatly. Complex
geometry (especially some things like helical sweeps which would be
needed for threads on screws or springs, if you have either) will
greatly increase the file size. I would expect an eDrawing with 200
unique parts and 500 total to be somewhere between 5 and 10 megabytes,
but it could be larger depending on configurations and complexity of
parts (as mentioned above). Also, if you have to embed the code for
viewing the eDrawing (making it a self-contained executable) it
increases the file size significantly, although not enormously. Have
the recipient download and install the eDrawings Viewer and you won't
have that problem.
3) Yes, SolidWorks has the analagous functionality in its drawing
package. Pretty easy to use and very flexible, once you get the hang of
it.
4) Don't believe you can turn layers on and off in import from DWG or
DXF, but you can handle that pretty easily by just making WBLOCKs of the
data you really do want. SolidWorks, like Inventor, generates drawings
from the 3D model, not the other way around, so typically what you want
to do with a DWG or DXF import is to create a PART, not a DRAWING
sketch. In so doing, layers are irrelevant. In making drawings (not
parts or assemblies) layers CAN be created for different type entities,
like dimensions, text and title block format lines. That's mostly
useful for exporting back out to DWG or DXF formats, for whatever
purpose you do that. For example, just like with AutoCAD naturally
sometimes you want to export just the object lines for use with CNC, and
so you want to be able to turn all the other layers off. You can do
that.
5) Yes, selection "windows" in all three environments work pretty much
just like AutoCAD. Drag from left to right and it's an include window,
right to left is a crossing window. SolidWorks doesn't have the other
fancier fence type selection methods or the type of filter selection
methods that AutoCAD has, but it does have a "Selection Filter" toolbar
which allows you to selectively filter such kinds of entities as Faces,
Edges, Vertices, Dimensions, Sketch Segments, Centerlines, Planes,
Datums, Weld Symbols, etc., etc..
'Sporky'
www.h2omarkdesign.com |
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TOP
Guest
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| Posted:
Wed Nov 30, 2005 9:10 am Post subject:
Re: Should I buy SOLIDWORKS? |
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I'd say all 5 are possible without too much difficulty. The drawing in
3 is not difficult at all but you might have to use a trick. 4 is not a
problem. 2D to 3D tools and dwg import will let you select layers and
fix up poorly drawn ACAD files. There is window selection though I dare
say this aspect may be used differently in SW.
I am not a big fan of edrawings. But others here are. You can section
and measure or not depending on how the file is saved.
If I understand 1 that would not be too difficult.
Now if you are well experienced in ACAD you may find crossing over to a
feature based parametric modeler a challenge. If you can forget ACAD
and approach SW with an open mind you will pick it up quickly.
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John Eric Voltin
Guest
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| Posted:
Wed Nov 30, 2005 9:10 am Post subject:
Re: Should I buy SOLIDWORKS? |
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The followup postings have answered most of your questions, but didn't
mention one detail regarding question 1. You can create a single part in
SolidWorks that contains four separate rectangles that are extruded to form
four separate bodies. Unfortunately, SolidWorks will not allow these four
rectangles to be butting together as you mention. Inventor will allow
rectangles to be butting and still extrude, but SolidWorks will not. Any
touching or overlap of the rectangles is not allowed in SolidWorks.
Otherwise the scenario you propose is possible within SolidWorks. You can
produce the desired result, but not with the method you described.
This particular topic is one area where Inventor is clearly superior to
SolidWorks. I hope that someday SolidWorks will duplicate this capability
since it reduces the need to trim sketches and improves efficiency. I
should note that Pro/E also has the ability to extrude touching or
overlaping sketch entities.
--
- John
John Eric Voltin
Mechanical Engineer
Agile Technology
512-633-0394
"Diemaker" <diemaker888@yahoo.com> wrote in message
news:1133322839.530404.173800@g43g2000cwa.googlegroups.com...
| Quote: | Should I buy SOLIDWORKS?
Long time user of acad, bought Inventor 4 years ago. It's improving
but so has SW it seems. And in my trade SW is becoming the norm... if
you can call a handful of 3d die designers the norm. But the top three
reasons SW is attractive is part configs, individual form control of
sheet metal, and edrawings. Very excited to see if configs can live up
to expectations. So I'm thinking about using my end of year money to
buy SW and have some questions. Oh, I'm foolish for not getting a 30
day trial, but too late now.
1 - I've been using master-sketching to control blocks that nest
against each other. If I understand correctly, in SW, sketch 4
squares,...2 butting, 2 gapped... extrude with one extrude. Then use
split feature to create 4 configs or 4 separate part numbers. Then
there is one file with 4 parts can be a sub in the assy. This would
effectively create a mastersketch, parts and sub within one file??? To
good to be true.
2 - Edrawings. I've only seen relatively small Edrawings. How is
performance with larger models, 200 unique parts, 500 total. Is it real
choppy? Can it be measured, sliced? How big would that file be, approx.
3 - Drawing side views. Dies are basically two halves, top and bottom.
It is common to show the bottom plan view with section lines to the
side views. Side views are a section of both top and bottom. In IV this
is possible with design views, plan view of "both halves" view is
section cut, then "both halves" plan view is replaced with
"bottom only" view, yet the side view still shows "both halves"
view. Does SW have an equivalent?
example: http://img507.imageshack.us/img507/2831/sideview5iv.jpg
4 - Importing a .dwg to the sketcher... can you turn layers on/off?
Widow select entities? Maybe even copy paste a dwg in a sketch? Or do
you have to import a whole file?
5 - Is there window selection in sketch environment? in model? In
drawing ?
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Sporkman
Guest
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| Posted:
Wed Nov 30, 2005 1:10 pm Post subject:
Re: Should I buy SOLIDWORKS? |
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I stand corrected on #4 as far as selecting layers on import goes. Paul
is right about that, now that I think back on it (haven't done it in a
while). The rest of what I said should be valid.
'Sporky'
TOP wrote:
| Quote: |
I'd say all 5 are possible without too much difficulty. The drawing in
3 is not difficult at all but you might have to use a trick. 4 is not a
problem. 2D to 3D tools and dwg import will let you select layers and
fix up poorly drawn ACAD files. There is window selection though I dare
say this aspect may be used differently in SW.
I am not a big fan of edrawings. But others here are. You can section
and measure or not depending on how the file is saved.
If I understand 1 that would not be too difficult.
Now if you are well experienced in ACAD you may find crossing over to a
feature based parametric modeler a challenge. If you can forget ACAD
and approach SW with an open mind you will pick it up quickly. |
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John Eric Voltin
Guest
|
| Posted:
Wed Nov 30, 2005 5:10 pm Post subject:
Re: Should I buy SOLIDWORKS? |
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Apparently, I was mistaken about SolidWorks having this limitation. This
morning I received an e-mail informing me of Contour Selection within
SolidWorks. While working on a sketch, right click in the graphics area and
choose Contour Select Tool. This will allow you to select the contours that
are used for the feature including touching or overlapping sketch entities.
It works quite nicely and I anticipate using it on a regular basis.
See the help file for complete details.
--
- John
John Eric Voltin
Mechanical Engineer
Agile Technology
512-633-0394
"John Eric Voltin" <jevoltin@agile-technology.com> wrote in message
news:O9bjf.17205$Au1.15214@tornado.texas.rr.com...
| Quote: | The followup postings have answered most of your questions, but didn't
mention one detail regarding question 1. You can create a single part in
SolidWorks that contains four separate rectangles that are extruded to
form four separate bodies. Unfortunately, SolidWorks will not allow these
four rectangles to be butting together as you mention. Inventor will
allow rectangles to be butting and still extrude, but SolidWorks will not.
Any touching or overlap of the rectangles is not allowed in SolidWorks.
Otherwise the scenario you propose is possible within SolidWorks. You can
produce the desired result, but not with the method you described.
This particular topic is one area where Inventor is clearly superior to
SolidWorks. I hope that someday SolidWorks will duplicate this capability
since it reduces the need to trim sketches and improves efficiency. I
should note that Pro/E also has the ability to extrude touching or
overlaping sketch entities.
--
- John
John Eric Voltin
Mechanical Engineer
Agile Technology
512-633-0394
"Diemaker" <diemaker888@yahoo.com> wrote in message
news:1133322839.530404.173800@g43g2000cwa.googlegroups.com...
Should I buy SOLIDWORKS?
Long time user of acad, bought Inventor 4 years ago. It's improving
but so has SW it seems. And in my trade SW is becoming the norm... if
you can call a handful of 3d die designers the norm. But the top three
reasons SW is attractive is part configs, individual form control of
sheet metal, and edrawings. Very excited to see if configs can live up
to expectations. So I'm thinking about using my end of year money to
buy SW and have some questions. Oh, I'm foolish for not getting a 30
day trial, but too late now.
1 - I've been using master-sketching to control blocks that nest
against each other. If I understand correctly, in SW, sketch 4
squares,...2 butting, 2 gapped... extrude with one extrude. Then use
split feature to create 4 configs or 4 separate part numbers. Then
there is one file with 4 parts can be a sub in the assy. This would
effectively create a mastersketch, parts and sub within one file??? To
good to be true.
2 - Edrawings. I've only seen relatively small Edrawings. How is
performance with larger models, 200 unique parts, 500 total. Is it real
choppy? Can it be measured, sliced? How big would that file be, approx.
3 - Drawing side views. Dies are basically two halves, top and bottom.
It is common to show the bottom plan view with section lines to the
side views. Side views are a section of both top and bottom. In IV this
is possible with design views, plan view of "both halves" view is
section cut, then "both halves" plan view is replaced with
"bottom only" view, yet the side view still shows "both halves"
view. Does SW have an equivalent?
example: http://img507.imageshack.us/img507/2831/sideview5iv.jpg
4 - Importing a .dwg to the sketcher... can you turn layers on/off?
Widow select entities? Maybe even copy paste a dwg in a sketch? Or do
you have to import a whole file?
5 - Is there window selection in sketch environment? in model? In
drawing ?
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Diemaker
Guest
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| Posted:
Wed Nov 30, 2005 5:10 pm Post subject:
Re: Should I buy SOLIDWORKS? |
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Thanks for reply, I do want this info. I've studied IV for 4 years.
Done real work with it. I know the differences/limitations of 3d. And
frankly, I see laying out tools in 2d then importing to 3d. 2d is
fluid, much easier to move a cut from one block to another. Much easier
to copy a portion of the design up 50" and draw in a different ideal,
then trash that ideal and move back the original. Dies are mostly flat
plates with openings and inserts that have to be arranged, 2d works
best for this. Call me stuck in my ways, but unless things in SW are
really different, I will still be using acad... And what could be
really different in SW is the configs. So I will belabor this.
Here is an example for question #1.
http://img326.imageshack.us/img326/7735/splitpart1zk.jpg
Can that one sketch be extruded, then split into the 7 different
blocks? Each block being a "config" that will be a separate item in
the BOM. I'm not familiar with "part configs" or the split
feature, so please be basic. You see #4 is gapped, or disjointed. Can
that still be split? #1,2,3 touch, but not with a straight line. Can a
split zig-zig and terminate? #5 &6 would be separate inserts inside
holes in #1. I made one rectangle and the other round corner to
complicate it. #7 is a block on top of another.
This duplicates what I call "master sketching" in IV. I create a
part file of just sketches, then derive into separate parts for
extruding. Change the master, the blocks change. Configs seem to make
this master sketching possible within one file. Maybe split isn't the
right approach, instead extrude the parts individually and make
configs. But the goal is to create multiple parts in one file that will
individually BOM and detail. So am I right on, asking for trouble or
completely dreaming? |
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Diemaker
Guest
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| Posted:
Wed Nov 30, 2005 5:10 pm Post subject:
Re: Should I buy SOLIDWORKS? |
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Good Edrawing info. The size is what I was hoping for. I believe SW
users get access to SW secure server for FTP of large files??? I
pictured the self-contained executable increasing the file by a
consistent size. Is this not so?
self-contained executable is a big plus since I would use edrawing
mostly for 3d design reviews with project managers, usually PM's have
broad band, but IT don't like special programs. And PM's don't
like updating software.
Scanning the board, seems some have problems with edrawing prints. But
models are reliable. I suppose there are all kinds of thing you can
draw on a print that might go wacky in an edrawing, Where as a model,
although complex, is consistent to translate. Does that rational sound
right? Things that go wack in an edrawing print are user blocks,
symbols, special tolerance or fancy fonts. The geometry, simple text
and dims are stable.
I could see edrawings a base for a paperless shop. |
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John Eric Voltin
Guest
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| Posted:
Wed Nov 30, 2005 5:10 pm Post subject:
Re: Should I buy SOLIDWORKS? |
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I stand corrected.
--
- John
John Eric Voltin
Mechanical Engineer
Agile Technology
512-633-0394
"Wayne Tiffany" <wayne.tiffanyRMVJUNK@asi.com> wrote in message
news:1133358999.9c149bc90cd0863022066d6868311f67@fe5.teranews.com...
| Quote: | Not quite true. You can have overlapping or touching sketches and extrude
separate bodies from them. The key is to use the contour selection tool
to pick the appropriate entities. If you uncheck the Merge box, then they
remain separate bodies.
WT
"John Eric Voltin" <jevoltin@agile-technology.com> wrote in message
news:O9bjf.17205$Au1.15214@tornado.texas.rr.com...
The followup postings have answered most of your questions, but didn't
mention one detail regarding question 1. You can create a single part in
SolidWorks that contains four separate rectangles that are extruded to
form four separate bodies. Unfortunately, SolidWorks will not allow
these four rectangles to be butting together as you mention. Inventor
will allow rectangles to be butting and still extrude, but SolidWorks
will not. Any touching or overlap of the rectangles is not allowed in
SolidWorks. Otherwise the scenario you propose is possible within
SolidWorks. You can produce the desired result, but not with the method
you described.
This particular topic is one area where Inventor is clearly superior to
SolidWorks. I hope that someday SolidWorks will duplicate this
capability since it reduces the need to trim sketches and improves
efficiency. I should note that Pro/E also has the ability to extrude
touching or overlaping sketch entities.
--
- John
John Eric Voltin
Mechanical Engineer
Agile Technology
512-633-0394
"Diemaker" <diemaker888@yahoo.com> wrote in message
news:1133322839.530404.173800@g43g2000cwa.googlegroups.com...
Should I buy SOLIDWORKS?
Long time user of acad, bought Inventor 4 years ago. It's improving
but so has SW it seems. And in my trade SW is becoming the norm... if
you can call a handful of 3d die designers the norm. But the top three
reasons SW is attractive is part configs, individual form control of
sheet metal, and edrawings. Very excited to see if configs can live up
to expectations. So I'm thinking about using my end of year money to
buy SW and have some questions. Oh, I'm foolish for not getting a 30
day trial, but too late now.
1 - I've been using master-sketching to control blocks that nest
against each other. If I understand correctly, in SW, sketch 4
squares,...2 butting, 2 gapped... extrude with one extrude. Then use
split feature to create 4 configs or 4 separate part numbers. Then
there is one file with 4 parts can be a sub in the assy. This would
effectively create a mastersketch, parts and sub within one file??? To
good to be true.
2 - Edrawings. I've only seen relatively small Edrawings. How is
performance with larger models, 200 unique parts, 500 total. Is it real
choppy? Can it be measured, sliced? How big would that file be, approx.
3 - Drawing side views. Dies are basically two halves, top and bottom.
It is common to show the bottom plan view with section lines to the
side views. Side views are a section of both top and bottom. In IV this
is possible with design views, plan view of "both halves" view is
section cut, then "both halves" plan view is replaced with
"bottom only" view, yet the side view still shows "both halves"
view. Does SW have an equivalent?
example: http://img507.imageshack.us/img507/2831/sideview5iv.jpg
4 - Importing a .dwg to the sketcher... can you turn layers on/off?
Widow select entities? Maybe even copy paste a dwg in a sketch? Or do
you have to import a whole file?
5 - Is there window selection in sketch environment? in model? In
drawing ?
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Rory
Guest
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| Posted:
Wed Nov 30, 2005 5:10 pm Post subject:
Re: Should I buy SOLIDWORKS? |
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? #1.... I've also used a master sketch in the assm to control multiple
retainers and trim steels. Change sizes in one sketch and it rebuilds
all the individual part files. Layout drawings in general are no
problem at all.
What part of the country are you located in if you don't mind me asking? |
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Wayne Tiffany
Guest
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| Posted:
Wed Nov 30, 2005 5:10 pm Post subject:
Re: Should I buy SOLIDWORKS? |
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Not quite true. You can have overlapping or touching sketches and extrude
separate bodies from them. The key is to use the contour selection tool to
pick the appropriate entities. If you uncheck the Merge box, then they
remain separate bodies.
WT
"John Eric Voltin" <jevoltin@agile-technology.com> wrote in message
news:O9bjf.17205$Au1.15214@tornado.texas.rr.com...
| Quote: | The followup postings have answered most of your questions, but didn't
mention one detail regarding question 1. You can create a single part in
SolidWorks that contains four separate rectangles that are extruded to
form four separate bodies. Unfortunately, SolidWorks will not allow these
four rectangles to be butting together as you mention. Inventor will
allow rectangles to be butting and still extrude, but SolidWorks will not.
Any touching or overlap of the rectangles is not allowed in SolidWorks.
Otherwise the scenario you propose is possible within SolidWorks. You can
produce the desired result, but not with the method you described.
This particular topic is one area where Inventor is clearly superior to
SolidWorks. I hope that someday SolidWorks will duplicate this capability
since it reduces the need to trim sketches and improves efficiency. I
should note that Pro/E also has the ability to extrude touching or
overlaping sketch entities.
--
- John
John Eric Voltin
Mechanical Engineer
Agile Technology
512-633-0394
"Diemaker" <diemaker888@yahoo.com> wrote in message
news:1133322839.530404.173800@g43g2000cwa.googlegroups.com...
Should I buy SOLIDWORKS?
Long time user of acad, bought Inventor 4 years ago. It's improving
but so has SW it seems. And in my trade SW is becoming the norm... if
you can call a handful of 3d die designers the norm. But the top three
reasons SW is attractive is part configs, individual form control of
sheet metal, and edrawings. Very excited to see if configs can live up
to expectations. So I'm thinking about using my end of year money to
buy SW and have some questions. Oh, I'm foolish for not getting a 30
day trial, but too late now.
1 - I've been using master-sketching to control blocks that nest
against each other. If I understand correctly, in SW, sketch 4
squares,...2 butting, 2 gapped... extrude with one extrude. Then use
split feature to create 4 configs or 4 separate part numbers. Then
there is one file with 4 parts can be a sub in the assy. This would
effectively create a mastersketch, parts and sub within one file??? To
good to be true.
2 - Edrawings. I've only seen relatively small Edrawings. How is
performance with larger models, 200 unique parts, 500 total. Is it real
choppy? Can it be measured, sliced? How big would that file be, approx.
3 - Drawing side views. Dies are basically two halves, top and bottom.
It is common to show the bottom plan view with section lines to the
side views. Side views are a section of both top and bottom. In IV this
is possible with design views, plan view of "both halves" view is
section cut, then "both halves" plan view is replaced with
"bottom only" view, yet the side view still shows "both halves"
view. Does SW have an equivalent?
example: http://img507.imageshack.us/img507/2831/sideview5iv.jpg
4 - Importing a .dwg to the sketcher... can you turn layers on/off?
Widow select entities? Maybe even copy paste a dwg in a sketch? Or do
you have to import a whole file?
5 - Is there window selection in sketch environment? in model? In
drawing ?
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Michael Eckstein
Guest
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| Posted:
Wed Nov 30, 2005 5:10 pm Post subject:
Re: Should I buy SOLIDWORKS? |
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Diemaker,
I am one of that "handful" of 3D die designers and I have sent a edrawings
proffesional file to your email, along with some comments. Take a
look. ------------I just looked at the file I sent, and I forgot to enable
the measure function. I will send a new file.
Good luck
Mike Eckstein
Tool Engineering Systems
"Diemaker" <diemaker888@yahoo.com> wrote in message
news:1133322839.530404.173800@g43g2000cwa.googlegroups.com...
| Quote: | Should I buy SOLIDWORKS?
Long time user of acad, bought Inventor 4 years ago. It's improving
but so has SW it seems. And in my trade SW is becoming the norm... if
you can call a handful of 3d die designers the norm. But the top three
reasons SW is attractive is part configs, individual form control of
sheet metal, and edrawings. Very excited to see if configs can live up
to expectations. So I'm thinking about using my end of year money to
buy SW and have some questions. Oh, I'm foolish for not getting a 30
day trial, but too late now.
1 - I've been using master-sketching to control blocks that nest
against each other. If I understand correctly, in SW, sketch 4
squares,...2 butting, 2 gapped... extrude with one extrude. Then use
split feature to create 4 configs or 4 separate part numbers. Then
there is one file with 4 parts can be a sub in the assy. This would
effectively create a mastersketch, parts and sub within one file??? To
good to be true.
2 - Edrawings. I've only seen relatively small Edrawings. How is
performance with larger models, 200 unique parts, 500 total. Is it real
choppy? Can it be measured, sliced? How big would that file be, approx.
3 - Drawing side views. Dies are basically two halves, top and bottom.
It is common to show the bottom plan view with section lines to the
side views. Side views are a section of both top and bottom. In IV this
is possible with design views, plan view of "both halves" view is
section cut, then "both halves" plan view is replaced with
"bottom only" view, yet the side view still shows "both halves"
view. Does SW have an equivalent?
example: http://img507.imageshack.us/img507/2831/sideview5iv.jpg
4 - Importing a .dwg to the sketcher... can you turn layers on/off?
Widow select entities? Maybe even copy paste a dwg in a sketch? Or do
you have to import a whole file?
5 - Is there window selection in sketch environment? in model? In
drawing ?
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John Eric Voltin
Guest
|
| Posted:
Wed Nov 30, 2005 5:10 pm Post subject:
Re: Should I buy SOLIDWORKS? |
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I have been testing this feature and I have not been able to create separate
adjoining bodies with a single extrude using the Contour Selection tool.
Merge does not appear to be an option within the context of a single
extrude. You can create two separate, adjoining extrusions and uncheck the
merge box to make them separate bodies.
Any suggestions?
--
- John
John Eric Voltin
Mechanical Engineer
Agile Technology
512-633-0394
"Wayne Tiffany" <wayne.tiffanyRMVJUNK@asi.com> wrote in message
news:1133358999.9c149bc90cd0863022066d6868311f67@fe5.teranews.com...
| Quote: | Not quite true. You can have overlapping or touching sketches and extrude
separate bodies from them. The key is to use the contour selection tool
to pick the appropriate entities. If you uncheck the Merge box, then they
remain separate bodies.
WT
"John Eric Voltin" <jevoltin@agile-technology.com> wrote in message
news:O9bjf.17205$Au1.15214@tornado.texas.rr.com...
The followup postings have answered most of your questions, but didn't
mention one detail regarding question 1. You can create a single part in
SolidWorks that contains four separate rectangles that are extruded to
form four separate bodies. Unfortunately, SolidWorks will not allow
these four rectangles to be butting together as you mention. Inventor
will allow rectangles to be butting and still extrude, but SolidWorks
will not. Any touching or overlap of the rectangles is not allowed in
SolidWorks. Otherwise the scenario you propose is possible within
SolidWorks. You can produce the desired result, but not with the method
you described.
This particular topic is one area where Inventor is clearly superior to
SolidWorks. I hope that someday SolidWorks will duplicate this
capability since it reduces the need to trim sketches and improves
efficiency. I should note that Pro/E also has the ability to extrude
touching or overlaping sketch entities.
--
- John
John Eric Voltin
Mechanical Engineer
Agile Technology
512-633-0394
"Diemaker" <diemaker888@yahoo.com> wrote in message
news:1133322839.530404.173800@g43g2000cwa.googlegroups.com...
Should I buy SOLIDWORKS?
Long time user of acad, bought Inventor 4 years ago. It's improving
but so has SW it seems. And in my trade SW is becoming the norm... if
you can call a handful of 3d die designers the norm. But the top three
reasons SW is attractive is part configs, individual form control of
sheet metal, and edrawings. Very excited to see if configs can live up
to expectations. So I'm thinking about using my end of year money to
buy SW and have some questions. Oh, I'm foolish for not getting a 30
day trial, but too late now.
1 - I've been using master-sketching to control blocks that nest
against each other. If I understand correctly, in SW, sketch 4
squares,...2 butting, 2 gapped... extrude with one extrude. Then use
split feature to create 4 configs or 4 separate part numbers. Then
there is one file with 4 parts can be a sub in the assy. This would
effectively create a mastersketch, parts and sub within one file??? To
good to be true.
2 - Edrawings. I've only seen relatively small Edrawings. How is
performance with larger models, 200 unique parts, 500 total. Is it real
choppy? Can it be measured, sliced? How big would that file be, approx.
3 - Drawing side views. Dies are basically two halves, top and bottom.
It is common to show the bottom plan view with section lines to the
side views. Side views are a section of both top and bottom. In IV this
is possible with design views, plan view of "both halves" view is
section cut, then "both halves" plan view is replaced with
"bottom only" view, yet the side view still shows "both halves"
view. Does SW have an equivalent?
example: http://img507.imageshack.us/img507/2831/sideview5iv.jpg
4 - Importing a .dwg to the sketcher... can you turn layers on/off?
Widow select entities? Maybe even copy paste a dwg in a sketch? Or do
you have to import a whole file?
5 - Is there window selection in sketch environment? in model? In
drawing ?
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Wayne Tiffany
Guest
|
| Posted:
Wed Nov 30, 2005 5:10 pm Post subject:
Re: Should I buy SOLIDWORKS? |
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No, what I did was 3 separate extrudes, each one picking its own contour.
Sorry if I mislead you.
WT
"John Eric Voltin" <jevoltin@agile-technology.com> wrote in message
news:zKijf.17284$Au1.5520@tornado.texas.rr.com...
| Quote: | I have been testing this feature and I have not been able to create
separate adjoining bodies with a single extrude using the Contour Selection
tool. Merge does not appear to be an option within the context of a single
extrude. You can create two separate, adjoining extrusions and uncheck the
merge box to make them separate bodies.
Any suggestions?
--
- John
John Eric Voltin
Mechanical Engineer
Agile Technology
512-633-0394
"Wayne Tiffany" <wayne.tiffanyRMVJUNK@asi.com> wrote in message
news:1133358999.9c149bc90cd0863022066d6868311f67@fe5.teranews.com...
Not quite true. You can have overlapping or touching sketches and
extrude separate bodies from them. The key is to use the contour
selection tool to pick the appropriate entities. If you uncheck the
Merge box, then they remain separate bodies.
WT
"John Eric Voltin" <jevoltin@agile-technology.com> wrote in message
news:O9bjf.17205$Au1.15214@tornado.texas.rr.com...
The followup postings have answered most of your questions, but didn't
mention one detail regarding question 1. You can create a single part
in SolidWorks that contains four separate rectangles that are extruded
to form four separate bodies. Unfortunately, SolidWorks will not allow
these four rectangles to be butting together as you mention. Inventor
will allow rectangles to be butting and still extrude, but SolidWorks
will not. Any touching or overlap of the rectangles is not allowed in
SolidWorks. Otherwise the scenario you propose is possible within
SolidWorks. You can produce the desired result, but not with the method
you described.
This particular topic is one area where Inventor is clearly superior to
SolidWorks. I hope that someday SolidWorks will duplicate this
capability since it reduces the need to trim sketches and improves
efficiency. I should note that Pro/E also has the ability to extrude
touching or overlaping sketch entities.
--
- John
John Eric Voltin
Mechanical Engineer
Agile Technology
512-633-0394
"Diemaker" <diemaker888@yahoo.com> wrote in message
news:1133322839.530404.173800@g43g2000cwa.googlegroups.com...
Should I buy SOLIDWORKS?
Long time user of acad, bought Inventor 4 years ago. It's improving
but so has SW it seems. And in my trade SW is becoming the norm... if
you can call a handful of 3d die designers the norm. But the top three
reasons SW is attractive is part configs, individual form control of
sheet metal, and edrawings. Very excited to see if configs can live up
to expectations. So I'm thinking about using my end of year money to
buy SW and have some questions. Oh, I'm foolish for not getting a 30
day trial, but too late now.
1 - I've been using master-sketching to control blocks that nest
against each other. If I understand correctly, in SW, sketch 4
squares,...2 butting, 2 gapped... extrude with one extrude. Then use
split feature to create 4 configs or 4 separate part numbers. Then
there is one file with 4 parts can be a sub in the assy. This would
effectively create a mastersketch, parts and sub within one file??? To
good to be true.
2 - Edrawings. I've only seen relatively small Edrawings. How is
performance with larger models, 200 unique parts, 500 total. Is it real
choppy? Can it be measured, sliced? How big would that file be, approx.
3 - Drawing side views. Dies are basically two halves, top and bottom.
It is common to show the bottom plan view with section lines to the
side views. Side views are a section of both top and bottom. In IV this
is possible with design views, plan view of "both halves" view is
section cut, then "both halves" plan view is replaced with
"bottom only" view, yet the side view still shows "both halves"
view. Does SW have an equivalent?
example: http://img507.imageshack.us/img507/2831/sideview5iv.jpg
4 - Importing a .dwg to the sketcher... can you turn layers on/off?
Widow select entities? Maybe even copy paste a dwg in a sketch? Or do
you have to import a whole file?
5 - Is there window selection in sketch environment? in model? In
drawing ?
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Diemaker
Guest
|
| Posted:
Wed Nov 30, 2005 9:10 pm Post subject:
Re: Should I buy SOLIDWORKS? |
|
|
Rory: Chicago. Sounds like you know what I'm talking about. Weaving
plates around each other, adjusting them as the design progresses or
revision hits. 2D die designers will always talk about how you can't
"stretch" in 3d. Master sketching is a way to achieve this. |
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