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gargoyle27
13th Jul 2010, 06:33 pm
i need to notate on an idw the length around a pipe (not linear length) from one leg to another and, from one hole to another, is there a way to do that?

i also can't get it to snap to the centre of the hole anyway, is there something i can do about that?

JD Mather
13th Jul 2010, 06:43 pm
There is an arc length dimension - but it seems you have three different questions here? Arc length. Length of pipe. One leg to another. One hole to another.

Can you attach your file here?

jdits7
13th Jul 2010, 06:58 pm
Not sure which version you are running but if you start with the dimension command and select the arc and then right click you have the option to either have arc length or loop length under the dimension type. Also to dimension to the center of a circle hover over the circle and the proceed to the center point of the circle and a green dot will appear that you can select. I am including a picture to show all three of these examples.

gargoyle27
13th Jul 2010, 07:25 pm
they are holes thru the pipe, so all you see is the cross section, but the dimension is around the pipe from the center of the hole to the feet, so i need that view to measure it

here is a picture

pinco pallino
14th Jul 2010, 06:38 am
It seems that you are trying to find the flat distance from the hole to the foot axis. I would consider a flat pattern on sheet metal.

gargoyle27
14th Jul 2010, 02:05 pm
its pipe tho, not rolled sheet metal

it might seem silly that i want a dimension like this, but this is what the welder wants

kencaz
14th Jul 2010, 02:58 pm
It's easy to get the distance. Find the circumference and divide by number of holes. I can see why he wants the dimension, however, that is pretty easy stuff and a welder should know how to find the distance.

KC

gargoyle27
14th Jul 2010, 03:02 pm
i know, i could even just put a note "evenly spaced" or something to that effect, but he wants it as an actual dimension

but i fiddled with the draft view and got it to work (or something that will work just as well)

thanks for all the help :D

pinco pallino
15th Jul 2010, 03:15 am
..that is pretty easy stuff and a welder should know how to find the distance.
I agree.
An easy lay-out is proper workmanship.
Your welder should learn how to do it right, rather then you adapting the drawing with wrong dimensioning.

Hopinc
15th Jul 2010, 10:18 am
I am really curious about this one as I cannot find anything in the dimensioning routines that allow me to detail the length of an arc. I can easily find the length of the arc between the holes by using measuring tools, but I cannot for the life of me get Inventor to dimension it either in model sketch mode or within a drawing. The only options I get are radius, diameter and angle dimensions.

Right clicking on the dimension type just does not give me the option described in Jdits7's post? Am I missing something here?

I have tried this in both 2010 and 2011 and looked it up in my rather old 2008 Inventor Essentials book without success.

Dave

JD Mather
15th Jul 2010, 11:50 am
I am really curious about this one as I cannot find anything in the dimensioning routines that allow me to detail the length of an arc.

Attach your file here.

Hopinc
15th Jul 2010, 01:06 pm
File as requested.

Dave

gargoyle27
15th Jul 2010, 02:19 pm
I still couldn't get the actual arc function to work, so i just replaced the degree measurement with the arc length, cheating sure, but it looks just fine on the drawing which is what matters most

and also, sometimes it doesn't matter what makes the most sense or is easiest, sometimes you just do what your told

on a side note, looks like i will actually be cutting threads on some pieces instead of using the thread tool, at least until it becomes more obvious how much it slows down the use of the full assemblies

Hopinc
15th Jul 2010, 02:54 pm
Hi Gargoyle27,

Unless you have quite a large number of thread cut parts I doubt you will see much difference in speed.

Attached is a very small example of an assembly of a condenser microphone capsule that I created some time back. As the threads on the capsule itself, the perspex locking ring and slug are all 40 TPI Brass Thread, plus the adjusting screws are 10 B.A., I had to cut these myself. I don't suppose it's something I would want to do for every screw thread but it does look good. Generally speaking I don't mind the simulated thread look, but on these small parts it was just not right.

If your boss is wanting to impress a customer with photo-realistic images or you haven't the time/inclination to add a new thread database then it has it uses.

Dave

MarkFlayler
15th Jul 2010, 03:26 pm
Is this what you were looking for?

I created some Work Axis and Work Points off those Axis to align your sketch better.

In the drawing I used "Get Model Sketches" by RMB on the part in the tree and then just used the Dimension command and switched to Arc.

Hopinc
15th Jul 2010, 03:47 pm
That's what I was trying to do Mark, but I am not sure about the original poster. I had gone several stages further and created the arc you see on the drawing plane by using f7, projecting the cut edges and adding a little sketch geometry. That's as far as I got as I could not find this arc dimensioning function.

BTW - "I created some Work Axis and Work Points off those Axis to align your sketch better." - I had removed all unnecessary geometry and your actions should not have been necessary.

And yes, your dimension is correct, although I was reading mine in metric at 44.975mm by dint of the measure command.

OK, I have got to the stage of applying the dimension as you have above, now using the annotate menu -where is this ARC selection in the dimension function??

Dave

MarkFlayler
15th Jul 2010, 03:55 pm
Start Dimension command, select the arc, then RMB before placing it. Select Arc Length

Hopinc
15th Jul 2010, 04:00 pm
Sorry Mark, those options do NOT appear in the RMB menu. Everything else does, but not the dimension type.

I suspect the original poster is seeing exactly what I am seeing. I also suspect you were thinking we are a bit dumb and that it should be obvious :-)


What version are you using?

Dave

MarkFlayler
15th Jul 2010, 04:07 pm
Are you getting the radius to appear first? If you get a green dot, then you won't get an option for this.

JD Mather
15th Jul 2010, 04:12 pm
Do not pick the endpoints of the arc - select the arc itself when dimensioning, then RMB....

gargoyle27
15th Jul 2010, 04:13 pm
I had the same problem, i didn't get the arc command in that menu

all i ended up doing was sketching on the drawing and dimensioning off that, and replacing the degree measurement with the length, normally i don't replace dimensions, but i didn't see any other way

and as far as the cut threads go, yes they do look better, but it was mostly about the head machinist not being familiar with the dotted line to indicate threads, so he wanted it to be more obvious on drawings, and i also have an older crumbier computer and i can see my assemblies getting weird and blocky after only having one or two cut thread pieces in it out of around 100 or so total pieces in the assembly

Hopinc
15th Jul 2010, 04:20 pm
J.D. - I was selecting the arc itself and not the end points. Mark you are not going to believe this, but I have just tried again and now the options are appearing under the RMB. ---- *#%# (expletive deleted).

I just don't get it??? I have done nothing different to what I have tried several times before. I knew that this dimensioning function should exist as I have used it in V.2009, but it just was not appearing.

Dave

Hopinc
15th Jul 2010, 04:29 pm
Mark, I owe you an appology and thanks, I have just discovered that the arc sketch in the model I posted was not on the true center of the extrusion. I have since adjusted it and followed your directions in your previous post. The only thing you missed in your instructions was the need to create a new sketch and project the arc geometry before applying the dimension - that actually worked this time and came up with the arc length option - go figure!

Dave

Hopinc
15th Jul 2010, 04:43 pm
Gargoyle27, I will attempt to explain how I got this to work.

First of all you need to create an offset horizontal plane through the centres of the holes. Create a sketch on the plane and project the cut edges. Create a circle directly over the outer projected circular. Trim the new circle so you have two short arcs between any two of the radial holes. Now draw axis lines from the mid points of these arcs to the centre of the extrusion.

Create another circle, exactly as you have just done and trim it to these axes, this is the true arc length between centres. Remove the two short arcs you created first.

Create your plan view in a drawing. RMB on the part name in the history tree and "Get model sketches." Once it has come through select the dotted edge of the drawing view border and create a new sketch. Project the arc. Select dimension and select the arc itself. As the radius appears move your cursor away slightly and press the RMB, the "Dimension Type" option should appear.

BTW - my apologies for hijacking your thread.

Regards all.

Dave

gargoyle27
15th Jul 2010, 05:02 pm
honestly, i have no idea what you just said, so i'm supposed to make new work planes in the iam and that will somehow translate to lines in the idw? i am a little baffled by this idea

i also don't know what a "plan view" or "history tree" is

keep in mind i have virtually zero formal training in inventor, everything i know i've learned over the past few months of fiddling, i know the basic functions inside and out, but not a lot more

don't worry about trying to explain it, i got what i did to work, so its all good

JD Mather
15th Jul 2010, 05:08 pm
Gargoyle27, I will attempt to explain how I got this to work.

First of all you need to create ....

Sounds like wayyyy too much work to me.

JD Mather
15th Jul 2010, 05:11 pm
... i am a little baffled by this idea...


Did I miss something, or did you ever post your file (as I suggested) in one of the two threads you started on different forums for this problem?

All I saw you post is image files. I am not familiar with editing image files in Inventor.

I suspect the idw approach would be trivially simple, if only I had a file.....

gargoyle27
15th Jul 2010, 05:14 pm
yes i also posted it on the autodesk website, i go by g_warner there, i saw you there too, and laughed to myself for a second

i have just been printscreening and pasting in paint and attaching jpgs, little easier than attaching a big iam with all the associated ipts (i don't have winzip)

JD Mather
15th Jul 2010, 05:23 pm
(i don't have winzip)

Windows XP, Vista, Windows 7 have built in compression.
In Windows Explorer right click on filename and select Send to Compressed (zipped) folder. (Actually you don't have to be in Explorer - but it is Explorer that does the zipping).

If the file is still too large drag the red End of Part marker to the top of the browser before saving and zipping with Windows Explorer.

gargoyle27
15th Jul 2010, 05:29 pm
oh ok, well i'll have to use that in the future, (at home i use winrar to (de)compress things and i can't install it as i don't have admin rights so i didn't think of that and i couldn't find winzip itself)

either way, i got the problem (essentially) solved, so i consider this particular matter closed :D

if you could help with my error issue it would be much appreciated

Hopinc
15th Jul 2010, 06:06 pm
Sorry for confusing you Gargoyle27, I assumed that you were more familiar with Inventor than you obviously are. As long as you have found a working solution that you are happy with that is all that matters at the end of the day.

J.D. - "wayyy too much work" - It took a lot longer to explain than it did to do, but even so time is money, so go on then let's hear your solution?

Dave