- Thread starter ajlelectronics
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I found an STL for the R32 but not one for the R33.
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Nissan Skyline R32 Cup Holder (IMPORTANT Read Summary) Updated by ace_305_ace
--------UPDATE (3)--------- Ok, so I printed the last .STL files I posted with a scaled down percent of 1-2% and it fit almost perfectly for me. so whichever file you may want to print MAKE sure you scale it down by at least 1-2% to have a good fit. Hope this helps! I uploaded pictures as well...
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ajlelectronics
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Fixed that for you! A far better method of imparting information.
Fixed that for you! A far better method of imparting information.
daedalusminos
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So we're designing an auto shift bezel....there's not enough detail to do a detailed design but I think this is the shifter:
...and I think it fits in this Honky Tonk mobile (sorry it's just what sprung to mind):
and the important bit:
Personally, since we're creating a totally custom part, I would make the bezel so it fitted in the rectangular pocket to make it more integral. However, that's not the brief, what we're trying to create is something like this:
Note that it has a slightly organic look with 3-way curves
...and I think it fits in this Honky Tonk mobile (sorry it's just what sprung to mind):
and the important bit:
Personally, since we're creating a totally custom part, I would make the bezel so it fitted in the rectangular pocket to make it more integral. However, that's not the brief, what we're trying to create is something like this:
Note that it has a slightly organic look with 3-way curves
ajlelectronics
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I have just spent a couple of hours on a Tutorial about F360 sketching. Lots and lots to remember but in all fairness I knew a lot of it already. Saying that it would be useful to draw one of those if I did not know some things already.
What it has not showed me yet is how to use sketches when I want to add bits later on. Its all well and good knowing everything you are going to need when you start but its often not like that. I am hoping that bit will be come clear soon.
I have to say I have watched a lot of tutorials and this is the best so far in how they get it across.
What it has not showed me yet is how to use sketches when I want to add bits later on. Its all well and good knowing everything you are going to need when you start but its often not like that. I am hoping that bit will be come clear soon.
I have to say I have watched a lot of tutorials and this is the best so far in how they get it across.
daedalusminos
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So let's get started, I made a fag packet sketch showing dimensions based (loosely) on the images above:
There are several ways to create the desired model with pros and cons to each, and I'll be deliberately making 'mistakes' and going through how to correct them.
The first method is to create a sketch and extrude it to form the model. So we need two trapeziums exactly per the fag packet sketch. There's no 'CREATE trapezium' option so we'll start with a rectangle and edit it to turn it into a trapezium. Start with a rectangle on the TOP plane 150 x 180 amd let's put the bottom left corner on the origin:
It's black which means it's fully constrained - it has defined dimensions, it's bottom left corner is anchored to the origin and because it's a rectangle the edges have horizontal/vertical constraints. We want a trapezium so we don't want the vertical constraints on the two vertical edges - we just select them and delete them, I'm also going to change the bottom dimension to 130 and add a dimension of 150 to the top line:
Notice three of the lines have gone blue (unconstrained) and it'd all gone a bit lopsided. The problem is that the middle of the top line is no longer vertically aligned to the middle of the bottom line. We can fix that by adding a construction line between the two mid points and adding a vertical constraint to the construction line:
Now it's looking pretty good but the 180 dimension is defining the length of the side (now at an angle) and not the distance between the top and bottom lines - easy to fix, just delete the dimension and add a new one defining distance between top and bottom and set to 180:
Now we need another trapezium within this one. We could offset this one and create another with a defined offset within this one but that may not be what the fag packet sketch defines - a quick check and I can see that the bottom offset on the fag packet is 15, which means the top is 180-140-15 = 25. So it's an uneven offset - also the trapezium angles may not match. Let's go ahead and construct the second trapezium using the offset and edit it to make it work. So I offset the outer trapezium by 15:
Note everything is black (fully constrained) and we can't do anything with the inner trapezium unless we break the offset constraint - select them and press DELETE. Now the inner trapezium is still constrained but with individual dimensions but only one of those is correct so we'll delete the other 3:
3 of the inner trapezium lines have turned blue meaning they are no longer constrained - we'll add the dimensions back in per the fag packet sketch. Something's not quite right, the two uprights are still blue and it looks as though the angle isn't quite right on the right side. In fact the same thing has happened as when we drew the first trapezium, we need to add the construction line between mid points and set it vertical.
Continued in next post...
There are several ways to create the desired model with pros and cons to each, and I'll be deliberately making 'mistakes' and going through how to correct them.
The first method is to create a sketch and extrude it to form the model. So we need two trapeziums exactly per the fag packet sketch. There's no 'CREATE trapezium' option so we'll start with a rectangle and edit it to turn it into a trapezium. Start with a rectangle on the TOP plane 150 x 180 amd let's put the bottom left corner on the origin:
It's black which means it's fully constrained - it has defined dimensions, it's bottom left corner is anchored to the origin and because it's a rectangle the edges have horizontal/vertical constraints. We want a trapezium so we don't want the vertical constraints on the two vertical edges - we just select them and delete them, I'm also going to change the bottom dimension to 130 and add a dimension of 150 to the top line:
Notice three of the lines have gone blue (unconstrained) and it'd all gone a bit lopsided. The problem is that the middle of the top line is no longer vertically aligned to the middle of the bottom line. We can fix that by adding a construction line between the two mid points and adding a vertical constraint to the construction line:
Now it's looking pretty good but the 180 dimension is defining the length of the side (now at an angle) and not the distance between the top and bottom lines - easy to fix, just delete the dimension and add a new one defining distance between top and bottom and set to 180:
Now we need another trapezium within this one. We could offset this one and create another with a defined offset within this one but that may not be what the fag packet sketch defines - a quick check and I can see that the bottom offset on the fag packet is 15, which means the top is 180-140-15 = 25. So it's an uneven offset - also the trapezium angles may not match. Let's go ahead and construct the second trapezium using the offset and edit it to make it work. So I offset the outer trapezium by 15:
Note everything is black (fully constrained) and we can't do anything with the inner trapezium unless we break the offset constraint - select them and press DELETE. Now the inner trapezium is still constrained but with individual dimensions but only one of those is correct so we'll delete the other 3:
3 of the inner trapezium lines have turned blue meaning they are no longer constrained - we'll add the dimensions back in per the fag packet sketch. Something's not quite right, the two uprights are still blue and it looks as though the angle isn't quite right on the right side. In fact the same thing has happened as when we drew the first trapezium, we need to add the construction line between mid points and set it vertical.
Continued in next post...
Onoff
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Yuk!
AutoCAD:
-Draw a rectangle 150w x 180h
-Draw a circle 130dia, mid point of the bottom of the rectangle
-Drag bottom corners to where they intersect with the circle
-Delete the circle
-Offset the (now) trapezium by 15mm
AutoCAD:
-Draw a rectangle 150w x 180h
-Draw a circle 130dia, mid point of the bottom of the rectangle
-Drag bottom corners to where they intersect with the circle
-Delete the circle
-Offset the (now) trapezium by 15mm
daedalusminos
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It now looks correct but the two uprights are still unconstrained, and even though it's OK to continue like this it's good practice to fully constrain the sketch to ensure the model is fully defined. Lets see what happens if we drag one of those uprights:
The inner trapezium moves horizontally, that's because we've only constrained it vertically by the 15mm dimension. We want the centre construction lines to be coincident - we do that by adding a coincident constraint between the mid point of the bottom line of the inner trapezium and the centre (construction) line of the outer trapezium:
That's it, fully dimensioned and constrained as per the fag packet. Later I'll go over another way to create the inner trapezium and there are also other ways to constrain the lines to achieve the same result.
daedalusminos
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We finish the sketch and we're returned to the main editing screen, notice that our sketching operation has appeared on the timeline:
Next we're going to extrude the area between the two trapeziums to create a solid - I'm going to assume the bezel is 40mm deep so we'll extrude it 40mm:
That's looking like the bezel we want but it's solid, we use the shell command on the bottom surface to create a model with 3mm thick 'shell'
That inner lip is too deep, we can select that face and offset it back up - 35mm (actually -35mm) should leave a 5mm return noite the timeline is filling up with our drawing operations Sketch, Extrude, Shell and Offset Face:
It all looks a bit square so lets fillet some of those edges. It's all gone a bit wrong, I've only selected the outer edges, the inner edges of the shell remain and it's cut into the body:
If we'd performed the filleting before the shelling then this wouldn't have happened, luckily we can just drag the fillet operation on the timeline to directly after the extrude. We can also double click the fillet operation on the timeline to edit it and add the outer corner fillets. If you get an error it's probably because the model cannot be created, in this case I reduce the top fillets from 15mm to 10mm:
The final step is to add the fillets for the cutout:
Continued in next post
Next we're going to extrude the area between the two trapeziums to create a solid - I'm going to assume the bezel is 40mm deep so we'll extrude it 40mm:
That's looking like the bezel we want but it's solid, we use the shell command on the bottom surface to create a model with 3mm thick 'shell'
That inner lip is too deep, we can select that face and offset it back up - 35mm (actually -35mm) should leave a 5mm return noite the timeline is filling up with our drawing operations Sketch, Extrude, Shell and Offset Face:
It all looks a bit square so lets fillet some of those edges. It's all gone a bit wrong, I've only selected the outer edges, the inner edges of the shell remain and it's cut into the body:
If we'd performed the filleting before the shelling then this wouldn't have happened, luckily we can just drag the fillet operation on the timeline to directly after the extrude. We can also double click the fillet operation on the timeline to edit it and add the outer corner fillets. If you get an error it's probably because the model cannot be created, in this case I reduce the top fillets from 15mm to 10mm:
The final step is to add the fillets for the cutout:
Continued in next post
Agroshield
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Miss, miss, are we allowed to ask questions as we go along?
In F360, can you type arithmetic expressions into dimension constraints? So above, could you type 180-140-15 into the dimension rather than working out the result as 25 and then typing it in?
I ask because doing so saves having a calculator in front of you and it also greatly reduces mistakes. Very often you need half of something, so typing 17.36/2 is the easiest way.
daedalusminos
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The completed model:
It's not bad but the sides are flat and just vertical, we can taper the extrude to give a bit more shape - this would also useful if we wanted to add a draft angle e.g. if this was the buck for a vacuum formed part - we just edit the extrude op on the timeline by double clicking. I've chosen 5 degree (entered as -5 to ensure it tapers in not out) taper, but that's broken the filet operation, the problem is there is no longer enough room for the size fillet we've chosen on the top edge:
I decided to change the taper and found that I could only get away with -1.5 degrees, you can see the fillets almost merging:
Let's go back to the sketch and demonstrate another way to create that inner trapezium - double click the sketch in the timeline and delete the inner trapezium - we can then copy the outer trapezium:
We can then edit the dimension for the second trapezium and add the 15mm bottom offset dimension - note that it's not fully constrained, we haven't set the horizontal position, we add a coincident constraint to the middle of the bottom line and the centre construction line of the outer trapezium:
Now finish the sketch and return to the model screen - oh dear that's well and truly broken it! Half the model is missing and I have some fillet errors:
Don't panic, we need to find out where's it gone wrong so let's roll back time by dragging the timeline pointer to just after the extrude (we know the sketch is good). That's not right, there should be a hole in the centre, so lets go ahead and double click on the extrude operation in the timeline and you can see that the inner section has also been selected for extrude - this probably happened when we deleted the inner trapezium. Easy to fix, just de-select the inner region:
Continued in next post...
It's not bad but the sides are flat and just vertical, we can taper the extrude to give a bit more shape - this would also useful if we wanted to add a draft angle e.g. if this was the buck for a vacuum formed part - we just edit the extrude op on the timeline by double clicking. I've chosen 5 degree (entered as -5 to ensure it tapers in not out) taper, but that's broken the filet operation, the problem is there is no longer enough room for the size fillet we've chosen on the top edge:
I decided to change the taper and found that I could only get away with -1.5 degrees, you can see the fillets almost merging:
Let's go back to the sketch and demonstrate another way to create that inner trapezium - double click the sketch in the timeline and delete the inner trapezium - we can then copy the outer trapezium:
We can then edit the dimension for the second trapezium and add the 15mm bottom offset dimension - note that it's not fully constrained, we haven't set the horizontal position, we add a coincident constraint to the middle of the bottom line and the centre construction line of the outer trapezium:
Now finish the sketch and return to the model screen - oh dear that's well and truly broken it! Half the model is missing and I have some fillet errors:
Don't panic, we need to find out where's it gone wrong so let's roll back time by dragging the timeline pointer to just after the extrude (we know the sketch is good). That's not right, there should be a hole in the centre, so lets go ahead and double click on the extrude operation in the timeline and you can see that the inner section has also been selected for extrude - this probably happened when we deleted the inner trapezium. Easy to fix, just de-select the inner region:
Continued in next post...
Misterg
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Yes
daedalusminos
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That looks better, we're still showing a warning on the fillet operation so let's drag the timeline pointer to just after that. We can see that the cutout fillets aren't working - that's because we deleted the trapezium they were associated with. Double click the fillet operation and we can see they've been deleted - easy just to add back in.
That's fixed that, no more errors on the timeline so lets forward to after the shell - that looks OK, let's move to the end of the timeline - that's not so good, the whole things too short!:
We'll open the offset face operation, and we can see it's selected both bottom faces not just the inner - that's easy just to de-deselect the outer one:
And that's it:
That's fixed that, no more errors on the timeline so lets forward to after the shell - that looks OK, let's move to the end of the timeline - that's not so good, the whole things too short!:
We'll open the offset face operation, and we can see it's selected both bottom faces not just the inner - that's easy just to de-deselect the outer one:
And that's it:
daedalusminos
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As @Misterg said yes you can, but it's better than that, you can refer to each dimension by it's variable name, here the 130mm dimension has been assigned variable name d1 (you can rename the variable names to be something more meaningful and add them to a parameter table:
But whilst I appreciate its better...it would confuse us beginners.
But this is the trap I keep falling into. To do that I need to learn too many things at the same time.
Its exactly what most of the youtube tutorials do... I used to teach basic PC computers when we had green screens at work. I soon learnt that I have to stop ASSUMING they understood what I was telling them..because if they didnt and it was often they soon got bored.
Onoff
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You'd have been better I think, measuring that with a Vernier.
