You are over defining your sketch. is there more to the video?
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SolidWorks is not Inventor and, therefore, works differently. I suspect that automatic relations are causing your problems. While sketching, you'll notice different icons next to your sketch tool; some white, some yellow. The white ones mean that SolidWorks is inferring a relationship, the yellow ones mean that SolidWorks is applying the relationship automatically.
Both SolidWorks and Inventor have automatically set relations.
In either way the relation is set automatically or manually, they are visible in
FeatureManager and visible in sketch if the relation visibility is turned on.
So I definitely know amount of relations of each object, for example
each of my blocks has just two relations as well as I have similar relations (constraints) in Inventor.
From looking at the video, you're grabbing three lines and attempting to make them vertical. However, one of those lines is already at an angle to the other two, that's why you're getting the error.
Not sure why you're using all those blocks as it seems inefficient, but I also don't know what your design intent is.
Jeff Mirisola wrote:
SolidWorks is not Inventor and, therefore, works differently. .
I teach both Inventor and SolidWorks.
I am not aware of any differences in sketch behavior.
I would not use the technique in attached *.sldprt file in Inventor or SolidWorks as I would consider poor sketch techniques. (I stopped even looking when I saw missing tangents in Block.)
I think the reason there are no tangents, is because they are "slot" sketch entities which do not require tangent relations to define. The fellow is obviously having issues with the sketch, regardless of how it was created. Possibly as a teacher of "both Inventor and Solidworks" you could supply some tips for Orest instead of hacking his technique.
Try turning off "snap to grid" and "automatic relations". Then go through your sketch and find the items that are not fully defined. I found them and created the relations manually and the sketch didn't over-define. For future sketching, try using sketch patterns and the hole wizard to create slots/hole features.
Hope this helps,
If the issue was that the square hole block was not holding it's shape, this information would be useful.
This hole was just exported from Inventor via the AutoCAD.
It is a training sketch. The task was about creating and placing blocks in special order.
I do not think the fully defined block geometry is the reason of sketch over defining.
This sketch is for training purposes only.
I did this project in Inventor and now I am going to create the similar things in
SolidWorks just to see how it works there.
I do not use the pattern at this case since it is a test of not even pattern features.
I mean let presume I would have just spreaded and repeated features, placed in not even pattern order.
I would say I would be lucky to have an even pattern but it rather an exception in real design.
(Of course I understand it is possible to make a pattern in this particular sketch.)
The reason of this sketch:
I have not even pattern holes on several depended parts.
Those parts are attached together so holes on corresponded parts must always match each other.
Those holes will be different in design and this hole design could be some special as those square holes.
For example those square holes are intended for welding special bolts and at other part there
will be corresponded slots.
The goal is: once I would change this special not even hole pattern at the one part
I will get the same changes at other one.
When I start projects I never know where my holes will eventually stop as I do some
alterations on a way to finished project.
For example in this project I had three-four level of depended parts which are different
in overall size but should always match each other.
Without making them depended from single sketch I should run between all of
them making the same changes.
And this manual way is also vulnerable for errors.
I see this way as natural, for example a puncture
machine with some special design of features will make the exactly same imprint
at the absolutely different details, so they will always match each other, and
this special holes could be done as fast as on a machine as on a depended part
If I would go by linked parameters I should
actually redesign the same sketch at other part drowning in bunch of linked parameters.
It may be easy just for really simple pattern.
There are a few ways to achieve this in SolidWorks. Holes series and derived sketches are options. I would simply make the pattern (equal or not) you want to be "driving" in one part and then add the other holes/slots/squares etc. while editing the adjacent part(s) in-context (editing the part in the assembly) and make the center points coincident. That way when you update the "driving" part it will change the "derived sketch". This could be done with blocks or the hole wizard.
Hope this helps, good luck with the transition,
I have tried this in-context way.
Quite unusual compare to Inventor, it has much more stuff in between to repeat the similar result.
Yes, if I would have blocks at the drive part it would be much easier to select required stuff
on driven part instead of Convert Entities of each hole.
But once again I should create some special pattern on the drive part.
It could be the similar pattern as causing over defined problems.
So far I step on all possible rakes to master this software.
I think it would be easier to start from scratch than to try everything to Inventor ...
Anyway thank you for good advices
You're welcome. Were you able to get that sketch to fully defined? I was able to do it by simply turning off automatic sketch relations and grid snaps then adding the last few relations manually.
As far as moving between different design software... I found when I went from SolidWorks to SolidEdge a few years ago, that it was a lot easier once I stopped trying to do things how SolidWorks software does. The var told me... They all can do similar things, they just speak different languages. So yes, starting from scratch might be easier. Cheers
Seems like this in-context feature may cause some troubles when both drive and driven parts
will be placed to different subassemblies.
I mean “Form new subassembly here” using driven and some other parts.
Did you ever placed driven part to subassembly?
Strange behavior. When I manually rotate the block, it is fine. When try to add vertical relation it is over defined. I used SketchXpert to find out what can be the reason and SW showed me that coincident relation of the leftmost bottom block is cousing it. So I deleted it and recreated. Very strange thing is that before adding coincident relation I had to force CTRL+Q. Otherwise SW showed me overdefined sketch.
In the attachment there is fixed sketch.
Drive Sketch3.zip 41.5 KB
At your sketch the middle top block has only coincident relation.
Once vertical relation is added and here is Over Defined error comes again.
It is quite inconvenient to find what is causing Under Defined sketch if it has blocks like this one.
In Inventor I can click on “Show All Degrees of Freedom” and it shows what exactly and how could move.
Could you please advise how you can find the Under Difined sketch stuff in SolidWorks?
Orest Yavtushenko wrote:
Could you please advise how you can find the Under Difined sketch stuff in SolidWorks?
Unless you've changed some settings, then fully defined lines will be black and under-defined lines, points, etc. will be blue in an active sketch.
Lines works well.
But what about blocks?
Seems like blocks do not change color, does not matter they are defined or not.
I don't use blocks at all, so I'm afraid I can't answer that.
I got the same problems.
I then deleted the bottom right hand block, then I inserted the block again. i then added the horizontal relation and then the coincident relation
It must be a bug in SW
I do design from scratch for all my projects.
For some designs I use blocks as it easy to spread some repeated written as blocks shapes, in not even order.
Also for some basic part designs it is much more vivid to draw most of shapes at same sketch,
as any further alteration will be mostly one shot- direct hit instead of clicking on numerous sequent features.
Projecting blocks (Converting Entities) is much convenient compare to clicking on each line of
shapes or groups of shapes from which they are composed.
I would emphasise I do it for some basic and not simple parts which will dictate the other parts or should accept
some standard parts fixture pattern.
For example there is a machine plate holding a bunch of custom and standard parts.
In Iventor I made much more complicated sketches than I am trying to build in SolidWorks.
So seems like Inventor is much powerful in this task?