Dimensions Flipped 1

[ecarr]

I have an assembly that I'm resizing and then saving the resized model in the Configuration Manager. If I change the model too much, some of my dimensions get flipped. For instance, if I have a hole that is dimensioned 1" to the right of a line and I resize the model, that dimension will now be 1" to the LEFT of the line.

Has anyone else experienced these problems? If so, is there any workaround/solution to this? I am going to be automating this modeling process to resize the assembly for SEVERAL models so I'm not able to check every single model and change the dimension as necessary.

 

[ctopher]

What version are you using? Are the dimensions flipping on the drawing also?
When you say you are resizing, are you just changing the sketch, or scaling the model?

Chris
Systems Analyst, I.S.
SolidWorks 06 4.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 06-21-06)

 

[wes616]

i have had this problem several times. The solution depends on how you have your model set up. Could you tell me how you have the holes. Are they sketch holes or generated through the hole wizzard. If they are sketch holes are they a seperate feature than the base part, or are they in the base sketch.



Wes C.
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[ecarr]

ctopher: I am using 2006 SP4.1. I do not have a drawing for these parts, but I'm assuming that they would be flipped as well. I have a top-level assembly sketch that I'm resizing which changes the components in the assembly.

wes616: The holes are created using Cut-Extrude. They are a separate feature than the sketch I am resizing.

 

[handleman]

You may have to adjust the way or order things are dimensioned. I've seen similar things happen before, especially as complexity increases. My guess is that during the rebuild process, SolidWorks remembers the absolute position of features, sticks them where they were prior to the rebuild, and then evaluates the constraints and dimensions. From your example, you have a hole that is 1" to the right of a line. That 1" is really just a distance value, with no specification of direction. If your line moves 1.5" to the right, then SW plops the hole in its original absolute position (now 0.5" left of the line). It then evaluates the 1" dimension from the line and finds that it needs to move the hole 0.5" further left to get it 1" away from the line. One workaround might be to dimension the hole from some different line that doesn't move. If it has to stay 1" to the right of the moving line then you could add an equation such that [hole dim]=[line dim]+1".

 

[ng89]

This happens to me all the time. Usually happens with either dimensions as you described or with tangent lines (curve is tangent to another line. change something unrelated and that curve "flips" 180 degrees so it is still tangent to the line, but in the wrong direction).

This is the single most annoying thing about SolidWorks to me. It makes it darn near impossible to use parametric models without have to re-check every single part.

Sorry I'm not much help, I just felt like venting, and letting you know it's not just you.

 

[ctopher]

I agree with handleman. I have seen this also.
I suggest turn in an enhancement request.

Chris
Systems Analyst, I.S.
SolidWorks 06 4.1/PDMWorks 06
AutoCAD 06
ctopher's home (updated 06-21-06)

 

[ecarr]

Thanks for the feedback! Good to know I'm not the only one with this problem.

handleman, I'll try your workaround but unfortunately I'm dimensioning to lines that aren't constrained using dimensions. This model is fairly complex as well. I'm setting it up to use an API that toggles relations and dimensions on and off so we can create the ~11,000 models for the job. So as you can see, there is now way we can individually check all the dimensions on all of these models.

Looks like I'll be turning in an enhancement request. I've never actually done that before. I'm assuming it's something you can do on the SW website?

 

[wes616]

eblack,

Here is something to think about (sorry if this is long winded).

When you are setting up your model, lets say for example that you are modeling a block with a hole a certain ED.

Do you fix one corner of the sketch to the origin, then sketch a rectangle dim it, and extrude, then put a new sketch on the surface and dim it the ED you need from the "free" edge.

If this is the case. you can drive the holes a couple of better ways.

1. dim your hole from the common (fixed) origin. If you are finding that you modify the same parts time and again, you can set up a series of equations to drive your features using this method. It takes a little more time, but pays off in the long run.

2. modify your original sketch to include the holes as part of the original sketch. Ths works best if you are creating a part with simple geometry

3. Try using the hole wizzard if you are creating standard sized holes. It seems to me to update feature changes better. This seems to me the best option if you have more complex geometry.

I have some more thoughts on this, but alas luch is over... let us know what your current solution is.

Wes C.
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[ng89]

handleman, I like your explanation and suggestion. Star for you.

I know for me, this happens alot more on very complex assemblies, and in the cases I can picture in my head, your explanation would make alot of sense. Unfortunately, the more complex the models, the harder it would be to implent your suggestion, but it's a good idea to think about anyway. It could come in handy sometimes.

 

[wes616]

I also tend to find that if you put a construction line "on-edge" or "colinear" to the edge, then dim from that construction line, the hole is evaluated properly.

Wes C.
------------------------------
No trees were killed in the sending of this message, but a large number of electrons were terribly inconvenienced.

 

[handleman]

eblackbu,
Remember, you can use reference dimensions in equations as well. You could create a reference dimension from the line to some fixed point and use that in your equation.

 

[CorBlimeyLimey]

handleman ... sorry but I have to disagree with your theory. Dimensioning feature from other features is the whole premise of Design Intent ... to ensure that the relationship of the feature being dimensioned remains constant when the model is changed.

I cannot remember ever having the OPs problem. I do remember dimensions flipping when rotating a feature through different quadrants of a circle, but that was a different problem. I tried to do what you described but couldn't recreate the problem.

I'm dimensioning to lines that aren't constrained using dimensions.

So am I correct in assuming that they are constrained using planes or other geometry?
If so then the problem lies within the application of locating for Design Intent. If the hole is to remain 1" from a certain edge, then dimension it from that edge or constrain it to a plane or geometry which has a 1" distance relationship to that edge. An equation will of course work, but seems to be a cumbersome way to achieve what should be a simple task.

FYI, a dimension can also be placed from a reference plane.

​

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[ecarr]

Thanks for the suggestions, wes616! I think the construction line method is what I want to do. I'm going to move/rotate this assembly around quite a bit in an area the size of a 90 story building. So as you can imagine, I'd rather not dimension to a global origin.

BTW, I'm also finding that the sketches I dimensioned to a top-level assembly plane update correctly.

I'll keep you posted as to what solutions I find work best!

 

[ecarr]

CorBlimeyLimey, I am dimensioning my hole to an edge that is changing and therein lies the problem. This doesn't happen EVERY time I resize the model and their doesn't seem to be a rhyme or reason as to why some dimensions flip and others don't. So it's hard to test out these various workarounds. But I do think that I have to do something more than just dimension to an edge because that's what I did originally.

...keep you posted.

 

[KingsPawn]

Hello all,I stumbled across this dimension flipping phenomena with the Hinge in the SW online Tutorial. This is obviously a simple part. In the tutorial you change the long dimension of the hinge by increasing it but not decreasing lower than the original value. On decreasing this extrusion below the original value, the hole locations fail since a dimension to the edge flips. I tried the on edge construction line method and the hole locations still fail when decreasing the long hinge dimension. HOWEVER, by redimensioning the hole locations to the plane of the left hinge face the parametrics hold together even when decreasing the long hinge dimension until the hole locations overlap.