First challenge: hole callout format.
The original drawing has some M4 metric holes with partial thread (it's not a through all thread, but only 15 mm deep):
When putting a DImXpert size dimension this information is missing:
It looks like the tap drill depth is missing.
I would have to manually add this piece of information with DimXpert and this would cause a little loss of time.
I submitted this issue to Dassault Systèmes.
Update from Dassault Systèmes:
This is a known current limitation in SOLIDWORKS, an enhancement request about this has been submitted in:
SPR 655649 - 'Ability to show thread depth in DimXpert dimensions'
I have run into the same issue and would like to see it resolved.
The second case is not a challenge, because I found a solution, but it's a useful piece of information for people that would step into the same case.
This is the deafult text position of the DimXpert size dimension for the threaded hole:
And this is where I change the text position as I want it:
I was wondering if there was a document option to set it deafult.
I tried to change document option for hole callout text style, but it had not effect. This was quite confusing because dimension is a hole callout (watch dimensions properties here):
So finally I found out that you have to change document options for diameter dimensions text style here:
So this makes me think that DimXpert size dimensions are not considered hole callouts but diameter dimensions.
This is the other challenge, reproducing this dimensioning scheme for the threaded hole pattern:
This will be a long comment, therefore I'm splitting it in two.
1 - Manual Dimensioning
When dimensioning hole diameter, horizontal dimensions, and 45 mm vertical dimension this is the result:
Some DimXpert value considerations:
- The 4 M4 hole pattern is automatically recognized (feature that generated hole was created with 4 points in one feature) and this would have not happened in a drawing when manually dimensioning the part (unless you used hole callout or dimxpert for drawings)
- The DimXpert manager shows manufaturing feature status; minus indicates that 3 holes are under-defined, while first hole is fully defined because there's the 45 mm vertical dimension. This would not happen on a 2D drawing
And here's a tought: in a 2D drawing I would be happy with the dimensiong you see in the first picture: I would suppose that people imply that 4 holes are aligned and their vertical distance is 45 mm.
In the 3D part I' not happy with the dimensioning scheme for two reasons:
- manufacturing feature is under-defined
- when clicking on the 45 mm dimension only one hole is highlighted, I need to transfer my design intent on the 3D PDF, and I want all the 4 holes to be highlihted.
By the way, I tried many ways to have the 45 mm location dimension recognize the pattern but I was unsuccesful. The final result is always the dimension to highlight only one hole.
Is there a way to have this manual location dimension point to the whole pattern ?
2 - Auto-dimension scheme
The auto-dimension scheme seems to solve the issue.
First: my dimension method is baseline, so I have to go to document properties and set this option (Dimension Method-Hole dimension-baseline):
Second, set these options for auto-dimension scheme:
So now I'm happy because:
- when clicking on the 45 mm dimension all holes are highlighted
- The manufacturing feature status is fully defined and colors also give a visual feedback
My considerations are:
- I've dimensioned the holes quicker than 2D drawing (I would have got the same result with dimxpert for drawings but people know or use it)
- I've got feedback about the manufacturing feature status
- I'm transfering design intent on the 3D PDF (visual feedback)
One suggestion for an improvement: the real part is complex and has some features dimensioned with baseline scheme and some with chain scheme. It is a little inconvenient to set the scheme in the document properties, it would be more convenient to have it in the auto-dimension scheme in order to decide in a case by case basis.
I've opened an enhancement request for this.
One last question (it's similar to the final question in the other post): is auto-dimension scheme the only way to have the 45 mm dimension highlight all four holes ?
Great posts, Alex.
Sorry I just got a bit time to look into these.
One quick thought on highlighting all holes: on identical annotations, DimXpert provides Combine Dimension and Break Dimension commands in the context menu like shown below. But it needs dimensions for all instances, which takes time, so Auto-Dimension may be faster.
Thank you Oboe for the suggestion.
Combine dimension is a great command to capture design intent in location dimensions. I liked it so much that I've created a video that shows it in action:
Next Step will be putting PMI for these additional holes:
The holes have been built is a single hole wizard feature:
The drawing shows two holes in the top view, and 4 holes in the detail view. Infact, if you use the callout anotation in the drawing, you'd have to force quantities (the drawing wrongly reports 6x in the top and in the detail view).
In DimXpert you have to plan accordingly.
I'll start from the holes in the top view.
I'll create a manual pattern for two of the holes:
In this case I have a chain dimensioning scheme, therefore I have to change my document options before using auto-dimension scheme: by setting chain method for holes:
Then I'll use the auto-dimension scheme.
I've lost my previous dimension placement!
I'll fix re-place my dimensions:
The hole pattern feature has no minus symblos, therefore it's fully defined, and when clicking on the 200 mm dimension both holes are highlighted.
In this case I would suggest voting for these enhancement requests, which would address this issues:
SPR 655657 - Ability to add dimensions to an existing DimXpert autodimension scheme ( auto dim dimension datum datums reselect )
SPR 664696 - Provide alignment options for DimXpert dimensions same as autodimension ( auto dimension dim left right top bottom align )
If I has not encountered this issue I would have said that dimensioning of this feature is much quicker than the drawing.
One last question: in many cases on 2D drawings you put some dimensions on the model because you have reduced space (like the 45 mm dimension on the picture above). The extension line inside the model is missing, is this expected behaviour ?
Now I'll take care of the other 4 holes on the deatil view.
I'll first create a manual pattern for the 4 holes:
I want to show those holes on a separate view (it would represent the detail view), therefore I'm creating a new annotation view:
I'll name it "Detail":
I'll use an auto-dimension scheme:
Consideration: hole pattern feature is completely defined, and there are less dimensions than 2D drawing. This indicates that my 2D drawing had redundant dimensions.
If I wanted to add the extra dimensions, this is what would happen:
DimXpert warns me that I'm over-constraining the part.
When adding the 35 mm dimension i'm over-defining the feature even more. This means that the dimension is not needed for the 4 holes.
OR: my interpretation is wrong: maybe customer wanted to take the midplane of the part as a refefence, and all other dimensions (10 mm) are not needed.
In MBD this misuderstanding would not be possible because the tool would just put the dimensions needed to constrain the manufacturing feature.
Or better, with GTOL auto-dimension scheme, it would have guided me by putting datums and positional tolerances to avoid any interpretation errors.
In this case I would solve the issue by adding reference dimensions:
Or, maybe, it makes more sense to me to take the midplane as secondary datum, therefore I decided to re-create the dimensions. And this is the result:
I'm creating less confusion because now it's clear that my datum is the midplane of the part, and the 10 mm dimensions are only reference dimensions (which would not be needed anyway).
This is the next case: a circular hole pattern:
So I will create an annotation view and use the auto-dimension scheme using these datums:
This is the result:
Question: how can the Hole pattern feature be fully defined if the threaded holes diameter is missing ?
I'll try to add it manually:
Question: It won't allow me to carry out operation, why ?
So I conclude that in order to workaround the issue I have to first put the diameter dimension of the 3 threaded holes, and then invoke the auto-dimension scheme. Result:
If I had to be honest here DimXpert could confuse user a lot. I submitted the issue to Dassault Systèmes.
Also, it seems that the only way to put the diameter and locaton dimensions of the circle through the center of the threee holes is using auto-dimension scheme. It's impossible to do it manually. This should be documented in a company MBD best pratice document.
Update for the isue: SPR 951780 “DimXpert Auto-dimension scheme incorrectly shows a hole pattern feature as fully defined “
Next feature: dimensioning the two counterbores.
This is the original drawing representation:
In my first attempt I'm having DimXpert recognize the two features as counterbores in my auto-dimension scheme:
My Datums are:
- mid-plane (magenta)
- purple planar surface
I'll then try to move the two callouts to a section view (I want to get the same representation as in the 2D drawing because I have some tolerances on the hole diameter dimensions):
I'll break the callout:
I'm missing the 27 mm hole depth dimension and the 35 mm diameter dimension.
I'll then choose another strategy, I'll recognize the two holes composing the counterbore as separate holes, therefore I'll create two manual patterns:
Larger holes pattern.
Smaller holes pattern.
I'll then create the same auto-dimension scheme as before, but this time I'm choosing the two separate pattern features as selected features:
Everyhting is defined, but the 45 mm dimension betwenn my secondary datum and the two holes is missing...
The DimXpert manager tree shows a "DistanceBetween8 Dimension", but it's not visible. It clearly refers to the missing dimension (the holes and part later faces highlight), but it's not there. When I right click on it a "Recreate pattern dimension" command appears, but nothing happens.
Finally I'm creating the section view, and this time the result is satisfactory.
So why is the 45 mm dimension missing ?
I've submitted the issue to Dassault Systèmes.
I went on testing other dimensioning schemes and sequences with plus/minus tolerances. I don't want to bore you with all the other challenges I steeped into like model features being under-defined or over-defined.
I've come to a conclusion:
- issue is caused by the way perspective customer uses dimensions, which is inconsistent and sometimes contradictory
- also, perspective customer doesn't use unique datums for dimensioning but in some views he uses certain datums, and in other views he uses other datums
See these examples. Datums in the top view:
Datums in te top view, which are different:
DimXpert was born for geoemtric dimensioning and tolerancing, which is, by defintion, a system in which all features are dimensioned respect to a fixed coordinate system that is defined by your datums. In that case there's no abiguity.
When using only Dimensional tolerances (plus/minus) there can be ambiguities when you're not consistent and always use different datums, therefore the system will have a hard time getting your manufacturing features either fully defined or over defined.
So my conclusion is that if you really want to go MBD you should "upgrade" the way you create PMI and use GD&T.
Great post with detail study on DimXpert features.
I used a part to reproduce some of your issues and these issues are indeed reproducible.
I am also glad that you found some work around such as Auto-Dimension scheme tool to resolve these issues.
Just like you said, some of the DimXpert issues really depends on how users define PMI or how they model the part in the first place.
I will take a closer look later and test if some of the remaining issues can be resolved by using a different approach of using DimXpert.
Thanks for sharing your thoughts!
DS Solidworks MBD Intern