I have a part where I used deform ( by point ) on my model but when I try to make drawing of that part i cant see that deform option.
Anyone have idea how to make it visible?
I wish I had an answer for you. I don't use the Deform feature, so have never run into this situation. Hopefully someone that's more familiar with it will be able to help. I don't know if this will do you any good, but it does show up in Shaded Views.
The only thing I can think of without more information is the possibility that there are multiple configurations, with the Deform feature suppressed in one, and that the drawing view is referencing this configuration. If that's not the case, can you post the Part and Drawing here?
File is in attachment.
I don`t know why but switching to Draft quality solves this problem.
May be because of this info from help:
Display states 'Available only if Display quality for new views is set to Draft quality'
What does SW mean under 'High quality' in this case?
i did that but nothing ... but if i change to shaded with edges...i can see it
To quote a post I read from Alin Vargatu yesterday, this is what
A SOLIDWORKS model has 3 major types of data that could be saved in the file and used in higher level assemblies and drawings:Feature Data: the recipe for building a part modelBody Data: the ideal geometry (math describing the geometry)Graphic Data: the triangular tessellation of this geometry that the user sees on the screen.High Quality Viewsextract information from the Body Data Set. That is why edges look perfect when printed or saved as PDF, when all drawing views are in High Quality state.are processed by CPU. That is why it takes a long time in some cases to get the edges computed.each model view, each section view and broken-out section view, require a separate set of Body Data to be loaded and processed!that is why recommended to use projected views and detail views as much as possibleeach configuration represented in a drawing view, require a separate set of Body Data to be loaded and processedthat is why is recommended to use Display States as much as possible instead of configurationsmulti core processing will be used when converting a Draft Quality View into a High Quality View. You will see a process called sldbgproc.exe appearing for each drawing view that is processed. I have not tested how many CPU cores could be used. On my machine I have 4 physical and 8 logical cores, and the maximum number of sldbgproc.exe processes I have ever seen running simultaneously was 3. Please reply if you can take advantage of more than 4 cores at a time.HQ Views are computation intensive, but require a smaller amount of data to be saved in the drawing file.the precision for dimensions is independent of the image quality settings.Draft Quality Viewsextract information from the Graphic Data Set. That is why sometimes edges look not ideal when printed or saved as PDF, when drawing views are in Draft Quality state.the Graphic Data was computed initially by the CPU, but once the data set is built, it is manipulated by the GPU. That is why is so fast, when you have a good video card.most of the time, the model has already the Graphic Data computed, before the drawing is created. That is what Draft Quality Views seem to update much faster than High Quality Views. There is no need to compute the ideal mathematical shape of the edges. Just use the triangles that were already computed.the Draft Quality drawing views tend to increase the drawing file size, since the tessellation is saved with the drawing.the precision of dimensions is dependent of the image quality settings (dimensions are attached to the triangles' nodes)an assembly containing a SpeedPaked sub-assembly will always be represented in Draft Quality Views
A SOLIDWORKS model has 3 major types of data that could be saved in the file and used in higher level assemblies and drawings:
High Quality Views
Draft Quality Views
The other one at the bottom that I refered to in my other post. It is related to the cosmetic thread.
Not quite sure though what could cause the problem to be honest..
Thank you very much for this information
That is very interesting. It shows up in a section view, but not projected views. Wow.
and here at this point, you can see from my cursor, that I can select it:
Whereas if I move my cursor out a little, it goes back to selection of the drawing view.
I would definitely show this on to your VAR.
changed to shaded with edges...i can see it lol
Even more interesting,,, If you increase the depth substantially it appears. I kept increasing the depth little by little then went from 10mm to 160mm
Is there another way to make this to avoid deform option?
You might possibly make it with a revolve and then add in the outside edges that are not round afterward:
I just thought of somet bug that I do get a lot. If you click on your flat pattern view that doesn't display the deformation and click over where the deformation should be, do you see the outline of the deformation? If so, you are probably suffering from the Crusty Old Template File Gotcha syndrome.
Refer to this thread : Drawing Views-Problem with updating
The form feature is not creating any tangent edges which would create display edges. Rotating the model with Zebra Stripes is mesmerizing. Curvature shows where it is located without revealing what it is.
As a workaround, go to your model and insert a sketch parallel to the view you want to show in the drawing. Create the silhouette using intersecting curve. In the drawing click the sketch and hit convert entities. Set the line weight in your layer or chose one for the sketch lines itself. It's still parametric if you change the deform.
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