sketch complex. how would you do that?

[marcof]

swx2010. . .

starting from an orthophotography I have to realize a series of channels excavated with "v" section according to a plot that is not manageable with repetitions, series etc. as each "island" enclosed between three or more lines along which run the channels is different from the others.
These islands are little less than 800 and the lines of course much more.
I have to decide how to best deal with this so I attach two test files that I did to make the idea of work.test grid channels_1.sldprt:on the basic extrusion I created the sketch "grille" (the one that will recalculate the orthophoto) then I made a series of extrusions up to the reference plane for the final thickness setting a sform angle equal to the middle of the channel angle. each extrusion is made with the option "selected contours" and choosing non adjacent regions. the reference sketch is shared for all 4 extrusions that create the finished part.test grid channels_2.sldprt:identical to the other to the "grille" sketch included. from here onwards I created a new sketch for every extrusion of the same "isole" by leaning on me to the sketch "grille"

Part 1 is reconstructed in about 0.6 sec while the 2 takes half the time.
In contrast to part 1 it is much, but much faster to realize because in the selection of the various regions you can see the preview and you can choose at best the islands to alternate, besides not having to redesign anything. in part 2 you have to draw once again an island without being able to see the preview.
I have made a variant of version 2 erasing all the relationships of the various sketches connected to the reference one so as to get many light sketches, as if I had drawn on the orthophoto the individual groups of islands and practically the recalculating times do not change but actually should not draw twice the same island (one in the basic sketch and the other to recalculate it)

As in the two examples placed the islands are 22 against the 800 that I should really do not want to find myself with biblical recalculating times for the increase of the complexity of the shared sketch, which I can only evaluate by doing so. on the other hand the idea of drawing on the orthophoto the various groups with an island at a time gives me the idea of a less immediateness in the possible modification or choice of groups of islands to extrude ogno vault

I add that the basic sketch or individual sketches of each extrusion will not be bound because they will recalculate an image. possibly I will put a "fix" for safety but to bind a sketch of that complexity with odds and angles is from delirium, also because it is a component that will not be reusable in other assemblies, and even if it were the changes would always be made on the basis of an orthophoto and could twist the sketch so as to make probable the failure of the connected features so it would probably be done from scratch every time.

I think I have provided all (or almost) the directions you need. At this point I ask you: how would you do the job? other ways to the one I took? how would you change my procedure and possibly which of the two would you adopt and why?

Thank you.

m.

 

[meccanicamg]

I think it makes more sense to work with the shared sketch between extrusion and the other. It's true that this 3d model will be unique. If you have to change the measurements, just change the main sketch. clearly if you add or remove cells. . It'll always be a mess.

I tried to make a tool to use by clicking only on the sketch, but apart from the errors that gives me swx... you need different constraints and in the end it weighs you not little. the useful thing is to do a piece at a time and suspend the first processing of the cells... so that time of the end you can fae all 800 cells. all the extrusions and go for a coffee and maybe take a trip to the block. But I don't see any other system to handle this. then if you are finished you can turn it into speed pack to use it faster.

 

[Pamak]

even if longer to load I would opt for method 1

If you change the grid, you will upgrade all extruded islands:finger:

to the limit if the loading time is too long creates 4 grids from 200 islands each

 

[re_solidworks]

swx2010. . .

starting from an orthophotography I have to realize a series of channels excavated with "v" section according to a plot that is not manageable with repetitions, series etc. as each "island" enclosed between three or more lines along which run the channels is different from the others.
These islands are little less than 800 and the lines of course much more.
I have to decide how to best deal with this so I attach two test files that I did to make the idea of work.test grid channels_1.sldprt:on the basic extrusion I created the sketch "grille" (the one that will recalculate the orthophoto) then I made a series of extrusions up to the reference plane for the final thickness setting a sform angle equal to the middle of the channel angle. each extrusion is made with the option "selected contours" and choosing non adjacent regions. the reference sketch is shared for all 4 extrusions that create the finished part.test grid channels_2.sldprt:identical to the other to the "grille" sketch included. from here onwards I created a new sketch for every extrusion of the same "isole" by leaning on me to the sketch "grille"

Part 1 is reconstructed in about 0.6 sec while the 2 takes half the time.
In contrast to part 1 it is much, but much faster to realize because in the selection of the various regions you can see the preview and you can choose at best the islands to alternate, besides not having to redesign anything. in part 2 you have to draw once again an island without being able to see the preview.
I have made a variant of version 2 erasing all the relationships of the various sketches connected to the reference one so as to get many light sketches, as if I had drawn on the orthophoto the individual groups of islands and practically the recalculating times do not change but actually should not draw twice the same island (one in the basic sketch and the other to recalculate it)

As in the two examples placed the islands are 22 against the 800 that I should really do not want to find myself with biblical recalculating times for the increase of the complexity of the shared sketch, which I can only evaluate by doing so. on the other hand the idea of drawing on the orthophoto the various groups with an island at a time gives me the idea of a less immediateness in the possible modification or choice of groups of islands to extrude ogno vault

I add that the basic sketch or individual sketches of each extrusion will not be bound because they will recalculate an image. possibly I will put a "fix" for safety but to bind a sketch of that complexity with odds and angles is from delirium, also because it is a component that will not be reusable in other assemblies, and even if it were the changes would always be made on the basis of an orthophoto and could twist the sketch so as to make probable the failure of the connected features so it would probably be done from scratch every time.

I think I have provided all (or almost) the directions you need. At this point I ask you: how would you do the job? other ways to the one I took? how would you change my procedure and possibly which of the two would you adopt and why?

Thank you.

m.

Hey, Marcof, good to see you around here. I have come to mind some ideas, one in particular seems good. I did so:

I took your part. I erased the extrusions and put it in an empty set.

I subsequently created (in a blank and new part) a rhombus-shaped sketch to use as a tool to cut the full and I saved it as a welding profile.

step 3 I created a blank part and I put it together. I went into the contextual modification of the part and I inserted the grid sketch as a derived sketch taking your grid sketch and the parallel plane.
after binding the sketch I entered a structural member who created the "male" of the quarries to be cut using the previously created section.
at this point I came out from the contextual modification of this part and I activated your original part and with the cavity function I created all the caves.
I have 2011 and leave you some pictures below...

Hi.

 

[re_solidworks]

I add: the beauty of my solution is that you can allow you to break the grid sketch in multiple sketches (if it becomes too complex) and in the "mask" part you can do more structural member functions if one becomes too complex.
Also you can change the cutting section to the flight and with the sketch derived in case of change of the grid you should not have big problems. . .

 

[SolidUser]

I'll give you another one without trying it.
do a sketch on the base plate that are the lines of your bases to v.
run the ribbing command on a box opposite your base plate.
run the command to dig the ribs with your base plate.

 

[Pamak]

Hey, Marcof, good to see you around here. I have come to mind some ideas, one in particular seems good. I did so:

I took your part. I erased the extrusions and put it in an empty set.

I subsequently created (in a blank and new part) a rhombus-shaped sketch to use as a tool to cut the full and I saved it as a welding profile.

step 3 I created a blank part and I put it together. I went into the contextual modification of the part and I inserted the grid sketch as a derived sketch taking your grid sketch and the parallel plane.
after binding the sketch I entered a structural member who created the "male" of the quarries to be cut using the previously created section.
at this point I came out from the contextual modification of this part and I activated your original part and with the cavity function I created all the caves.
I have 2011 and leave you some pictures below...

Hi.

so doing cuts everything following the path of the grill

from what I have understood to him serves to group of the islands (or maybe I got it wrong)

 

[Fulvio Romano]

starting from an orthophotography I have to realize a series of channels excavated with "v" section according to a plot that is not manageable with repetitions, series etc. as each "island" enclosed between three or more lines along which run the channels is different from the others.

Is it a penrose tipping?

 

[cacciatorino]

not to be provocative, but did you think to draw it in 2d and then give the miller the typical section of the tool and a nice dxf?

 

[marcof]

the useful thing is to do a piece at a time and suspend the first processing of the cells... so that time of the end you can fae all 800 cells.

If I use my method with the shared sketch I have to force keep all the extrusions activated otherwise I have no way to know what they have already been done and what not. it is necessary to select alternating them otherwise they are connected to each other and the v channel does not form. So if I have the "islets" 1,2,3,4,5,6,7.... I must first select 1.3,5,7 then 2,4,6. as the design is complex if I do not see what I have already extruded I do not come out.
Hello and thank you

 

[marcof]

(cut)
step 3 I created a blank part and I put it together. I went into the contextual modification of the part and I inserted the grid sketch as a derived sketch taking your grid sketch and the parallel plane.
after binding the sketch I entered a structural member who created the "male" of the quarries to be cut using the previously created section.

It really seems to me a great solution, to which I would certainly not have come because I never use structural members and these are workarounds by hulled people who can exploit certain features that know well for unusual work
I have tried but I have to understand how the selection of sketch lines works because once I choose my rombo profile I can select a few lines of all the sketch and for later I have to do a "new group" and anyway I did not understand the logic with which either accepts a line to insert the structural member. I hoped it would be enough to select all the sketch with the grill
I will work on this weekend and I will now use the structural members for a lot of useful things with custom profiles :finger:

Hello and thank you!

 

[marcof]

I'll give you another one without trying it.
do a sketch on the base plate that are the lines of your bases to v.
run the ribbing command on a box opposite your base plate.
run the command to dig the ribs with your base plate.

I'm not sure I understand well, but I look at the nervature command that I never used, then I ask you some more sensible questions than I could ask you now.

Is it a penrose tipping?

No, no, nothing so intriguing

not to be provocative, but did you think to draw it in 2d and then give the miller the typical section of the tool and a nice dxf?

In fact, I just have to make the 3d of an existing object. right for chatting, those v excavations are handmade and fresandolo would not be possible to get the living edges at the end of excavation or on the outer sides of the zig-zag routes.

hello and thanks to all for the interventions

 

[re_solidworks]

It really seems to me a great solution, to which I would certainly not have come because I never use structural members and these are workarounds by hulled people who can exploit certain features that know well for unusual work
I have tried but I have to understand how the selection of sketch lines works because once I choose my rombo profile I can select a few lines of all the sketch and for later I have to do a "new group" and anyway I did not understand the logic with which either accepts a line to insert the structural member. I hoped it would be enough to select all the sketch with the grill
I will work on this weekend and I will now use the structural members for a lot of useful things with custom profiles :finger:

Hello and thank you!

Hi.

logic is quite simple. you can gather in the same group segments that form a continuous profile (also closed) or parallel elements.
Maybe I'll do it again with 2009 (which I still have) so you see how I created the groups.
basically I did the perimeter, then the existing continuous contours (as much as possible) and then the lines not parallel or usual with others.
Keep in mind that the profiles are automatically trimmed into the same funznion as a structural member, leaving entire groups inserted first. this in principle is logic... .

Hi.

 

[marcof]

Hi.

logic is quite simple. you can gather in the same group segments that form a continuous profile (also closed) or parallel elements.
Maybe I'll do it again with 2009 (which I still have) so you see how I created the groups.
basically I did the perimeter, then the existing continuous contours (as much as possible) and then the lines not parallel or usual with others.
Keep in mind that the profiles are automatically trimmed into the same funznion as a structural member, leaving entire groups inserted first. this in principle is logic... .

Okay, clear, thank you very much.
don't waste time to remake the part in 2009. I work with calm and if I have insurmountable difficulties I will make myself alive

Hi.

 

[re_solidworks]

Okay, clear, thank you very much.
don't waste time to remake the part in 2009. I work with calm and if I have insurmountable difficulties I will make myself alive

Hi.

Okay, try it yourself, eventually it's pretty intuitive.