I have a copy of 750 dxf files for most of the Australian Standard steel sections and use these to create parts in assemblies. I would prefer not to use the part library as there is a lot of work in parameterising each part. The only way I have found to import dxf files finishes up with a ZW3D part with no sketch, just a curve list so that I cannot use External Sketch Import to use the part in another job file. Is there a better way? It is desirable to create a new part in each root file rather than referencing one part in another file so that changes in one job do not affect other jobs.
Jim
Hi Jim, interesting question.
I have a client who has converted over 2,000 DXFs to 3D parts over time.
I guess there is no point converting anymore than you need so the task may not be too onerous.
My process is to import the DXF then use Move to locate the wireframe components on the correct origin.
Then a sketch over the top and reference the relevant curves. Unlink and convert to functional(non construction)curves. I use the trim/extend command to make the segment joins, then the auto constrain to lock it up. Although unless you are modifying the profile this might be overkill.
Then I delete the wireframe - turn off the wires.
You can also build your own weldment profiles - theres a how to instruction somewhere.
And you can config a fully constrained and dimension ed profile to change size as required via a config table.
Then there’s sketch blocks which can bypass the constrain process - take unlinked reference curves and block them. Blocking locked them up. They can be positioned by constraints with a sketch then and used any time.
So that’s the starting point.
Actually I didn’t know there where than many profiles!
Cheers
Paul
Utilities/Recover Faces with Encapsulate History sometimes converts a wireframe to a sketch. I have used the same process of sketching over lines to create sketches and just create a few as needed so that it does not become a chore. You need to put in a surprising number of constraints for rectangular hollow steel sections to keep their shape if using a config table to scale sizes. My aim is to build a library of 3D parts of steel sections for use in various projects. These are not weldments and anyway Australian sections are slightly different from ISO sections as we have some metric sections rounded from historic imperial sections. I will give sketch blocks a try. Thanks
Jim
Hi Jim,
interesting solution re the Encapsulate.
So you use Auto Constrain - filtered control?
Just a note re sketch blocks. They are not well documented.
But some tips I have recently learnt.
You can grab a sketch block from any file. If you keep it linked the original stays in the parent file.
This means it can only edited in that file. To do this you need to know which file it lives in as there is no way of backtracking.
If you Unlink during insertion - the block becomes a local copy and can be edited without changing the parent. It will have the same name but be independent.
Cheers
Paul
Paul
I do not use auto constrain as it does not always pick up the critical constraints and sometimes over constrains. For example with rectangular hollow sections, the radius on the outer corners and the radius on the inner corners must have a common centre but auto constrain tends to dimension the flat sides and then the radii without constraining them to concentric and it all blows up when you scale the sketch. I find it better to get the radii concentric, the inner and outer sides vertical or horizontal then dimension one vertical and one horizontal side and the thickness of the sides which is more reliable. I do use import sketch - unlink where the original part is from a sketch not a wireframe and this saves time.
Thanks
Jim
Hi Jim,
Auto constrain allows for choice of constraints to be applied and order.
Although sometime by the time you have set the filters etc, you might have manually constrained anyway.
You realise that you may not need inner and outer profiles don’t you?
Thicken option in extrude can take care of the thickness.
Cheers
Paul
No Paul, of course I didn’t notice the thicken option. There get to be so many tricks in this type of software that some get missed. I could always read all the help file but life is too short and this is where co-operation between users like this excellent forum is valuable. Thanks again for your help, this will save time and may make reuse of parameterised sketches for hollow sections a practical option. More learning to be carried out.
Jim
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Neat! I sure will make use of that :P.
Nicolas