Compound Angle on Frame Member

[BillB]

O.k. Guys, here's a GOOD un,

 

Per the attached images, I am trying to add a 4" x 2" steel member along the edge of the purple line (constrained) from the yellow attachment plate to the front brown "L" brackets. This member will be on both sides of the frame and is running at a compound angle. Really having a couple of problems with this:

 

1. After doing the sketch on the Work Plane and exiting sketch I then go to the Frame Generator to Insert Member, BUT I can not pick the sketched constrained line, acts like it's not there. The cursor WILL highlight lines on the yellow attachment bracket, brown "L" brackets, ect. but not the red and gray

parts of the frame. ---- What did I do wrong?

 

 

 

2. I am not sure how to go about getting the Work Plane exactly where I need it. Per the one image I really need the contrained line over about 1/2".

I knew I would run into this problem one day, inserting a member at a compound angle at precise dimensions.

 

Any help, suggestions, shouting words of encouragement would be GREATLY appreciated.

 

BillB

[shift1313]

to answer your questions backwards, you can start a 3dsketch. When starting a sketch there is a drop down box, you will have 2d sketch and 3d sketch. When doing a 3d sketch you can constrain lines to planes or you can "free" sketch in 3d. Before you start sketching if you project geometry you can include those dashed reference lines and snap to their intersection point.

 

To create a plane you can do a few things. a reference plane(one you created or xy,xz,yz) and a line will let you rotate a plane about an angle. 3 points will give you a plane as well. you could select the dashed line intersection, another point on the vertical line and the point on the other end of your line to create a plane there.

 

For getting that sketch to become active id have to play around with it. If you right click on the sketch that consumes that line in your design tree on the left you should be able to select a few things. I cant remember if its "adaptive" in inventor that will allow you to share that sketch. I havent had an issue with lines not being selectable in frame generator before.

 

can you post a screen shot of your design tree with the sketch that shows that line and your frame generator so i can see the heicharcy. can you also right click on that sketch in the design tree before you Print Screen.

[BillB]

Howdy again Matt,

 

Not sure what the problem is but when I go to the Sketch drop down in the Menu Bar all that's available is 2D Sketch, the 3D is grayed out. That's what i thought I could do until I saw that. Let me get some screen shots and I will get them on here in a short while

 

Thanks

 

BillB

[BillB]

Hey Matt,

 

O.k., here's the screen shots I think you wanted to see. Sketch 9 shows the constrained line on the Work Plane, this was the one that I was going to use for placing the 4x2 member edge on. Sketch 10 shows the Construction line and Center Point that I placed on the face of the brown "L" bracket, I actually wanted the end of the constrained line to go to the Center Point. Not sure if I did some procedures wrong or what.

 

Thanks

 

BillB

[BillB]

Here's the one with Sketch 9 with RMB, hope it helps

 

BillB

[shift1313]

bill, is the vertical line in sketch 9 a construction line?

 

also when you are creating frame members there is a grid with a bunch of "dots". these dots allow you to place the frame member using different points. for instance if your "guide" line was to be the top left corner, you could select that "dot" on the creation pop up window where you pick the size and so on.

 

 

since i only have inventor 11 in front of me my windows and layout is going to look a bit different than your setup but your design tree doesnt look as it should(to me). Hopefully mark or someone with more frame generator experience will chime in.

 

Basically the issue i see is extrusions and sketches not contained in a part, but rather in the assmbly(if that makes sense). Here are a few screen shots for you from an older version.

 

The first pic is the model tree in the assembly environment. The only thing seen is the name of the components. If i were to expand them(+) you would only see mates applied to them. The second pic is in part mode(right click on the HUB:1 component and Edit). This shows you the features, their sketches and planes and so forth. The third pic shows you right clicking on the sketch. In this version of inventor i have a Share Sketch options which allows me to use it with other components in the assembly. I cant remember if this terminology or process changes with the newer versions.

[BillB]

Hey Matt,

 

O.k., the slightly angled vertical line is an extension line of a dimension (see top image). The shorter vertical line is a Projected edge off the "L" bracket. Yes, when I Insert frame members I use the "dots" for locating the edges. That's how I did the red and gray parts of the frame in the images. Yeah, I'm wondering if I didn't screw up on how I went about the assembly of the "Frame" and other components

[BillB]

Here are some screen shots of the Model Tree, hope they help.

 

BillB

 

Sorry guys,,, there too small, I'll try again

[BillB]

Hope these come out better.

 

BillB

[shift1313]

sorry bill i didnt get a chance to play with this at all this weekend. I should get a chance to try something tonight(i hope).

[BillB]

Hey Matt,,,, not a problem at all. I appreciate you taking the time to look. Maybe you should kick back and have a couple of cold one's. I looked at it a little this weekend but I sure didn't have any epiphanies ( wow,,,,haven't used that word before,,, or would that count????)

 

Take care and have a good one.

 

BillB

[shift1313]

alright bill i played around with it a bit and i cant seem to reproduce the problem you have. I think the issue is all in how you setup/model everything. I made a bunch of screen shots that ill try to explain here. First off i tried to recreate some of your frame that is being used for this part.

 

In the image below i already had the frame members drawn then i started a new component which I called FramePath2. Framepath1 was used to create the base. Now FramePath2 really isnt necessary the way I drew it because I could have just used the edge points for my frame member path and produce the same results.

 

 

I added some notes on this one.

 

 

Here you can see the frame member pop up window and what "button" i selected in the window for my path. You can always look at the preview and see if the orientation is correct. I know you were using 2x4 but i just used 2x2 since it was already selected:)

 

 

 

since that really could have been done without the sketch i went back and created another component which I called framepath3. This was a 3d sketch out in space that didnt touch any frame member just so there were no issues. I finished the sketch, went back out into my assembly and added another frame member.

 

 

this worked fine with no issues as well.

 

 

i also uploaded a picture of my model tree. im going to do one more thing and upload some more screen shots.

[shift1313]

Okay bill. What i did here was create a frame member that was based off my two plates but not using any end points as my path.

 

First thing i did was create a new component called framepath4. This time i didnt use any 3d sketches, only 2d. First i start by exiting out of the sketch it starts you in and deleting it. Then i start a new sketch selecting my front plate as a plane. This will create an Adaptive work plane and an adaptive sketch that are based off this feature. I use the Project Geometry button to project the top and left edge of my plate. Then i create a point and position it using Dimension.

 

 

I finish that sketch and follow the same procedure on the other L bracket. This again makes an adaptive work plane and sketch.

 

 

you can see in this pic my two points(circled) and you can also see the dark red projected geometry lines. I turned the visibility of the work planes off cause they are annoying to look at:)

 

 

Now i exit my part and go back into the assembly. Insert a frame member and use those two points as my endpoints.

 

 

note that using this method left the tubing orientation off. I used the rotate option to fix it.

 

After that i used the trim/extend option to get the square tube out to both of those plates.

 

 

 

 

I think the most important thing here is how you create these assemblies and the sketches you use to define paths. I think because you are creating sketches in the assemblies and not as their own components that it may be giving you trouble. I try not to reference other components when possible. For instance if i had two plates that bolted together, i wouldnt project the holes from one plate to the other, i would redraw and dimension the second plate.

 

Im not sure if my method is good or right, but hopefully it at least gave you something to think about.

[BillB]

Wow Matt, that's a lot of work you did there, I hope you know I really want to thank you for the help and guidance. I kind of got the gist of what your saying but I will have to study it a while longer and try the suggestions you did. Being an Inventor Newbie some of the work you did is a little new to me, but I will wade through it.

 

I will let you know how it works out at this end.

 

Thanks again Matt, you have a great day

 

BillB

[BillB]

Hey Matt,

This is what I came up with after following what you did in Post #13,,, kind of. Wasn't sure what this procedure was for "" First i start by exiting out of the sketch it starts you in and deleting it. Then i start a new sketch selecting my front plate as a plane. This will create an Adaptive work plane and an adaptive sketch that are based off this feature."". Am I missing something? Here are a couple of screenshots, one of my Model Tree and one of the Frame, see what you think.

 

Thanks Again Matt

 

BillB

[shift1313]

no problem bill. it didnt really take that long. it takes long to type and make screen shots really.

 

out of curiosity, what is the frame for?

[BillB]

Matt, It's for a Brush Hog that's for a Skid Steer Unit (Bobcat)

 

BillB

[shift1313]

thats pretty neat bill. I see the drive shaft guard and the pto drive now.

 

The part you underlined there. When i create a new part i just click out in the screen somewhere and I dont select any existing parts. This creates a new sketch automatically that is just out in the air somewhere. This is habit for me because i try not to create any adaptive planes right off the bat. Unless its absolutely necessary for me i avoid adaptive parts. They are fine to use but you really have to understand the implications of adaptive parts and referencing other components/planes outside of your part. In my mind its better not to if you can avoid it but that doesnt work for every industry/situation. There are housings I design where(in other software) will project my geometry, dimension it and then break all ties with other components.

 

 

everything is looking good. the only things in your model tree that worry me are Sketch6 and Extrusion 1 and 2.

[BillB]

Hey, thanks Matt, Yeah, this unit actually runs off of a hydraulic motor and then it couples to a 90* Angle Drive. The Skid Steer don't have a conventional PTO, so to speak.

 

That's a good tip to know about the Sketch and Adaptive, I'll start using that myself (when I get my head wrapped around it a little better)

 

The Extrusion1 and Extrusion2 was the way I was able to trim the ends of those 6"x2" rect. members that I was having trouble with in my other Post, probably not right but I wanted a way to trim without making a separate part to trim to. (Although I did cap them later as you can see in the below image)

 

Thanks again Matt, really appreciate it.

 

BillB

[shift1313]

i see the other drive now:)

 

yeah since you capped those i would use that feature to extend/trim your square tube. If you right click on those extrusions in the model tree and suppress them you will probably get an error(if you used that to draw your cap) but there are work arounds for it now. If i get the chance tonight ill draw up a frame member and try to trim the end of it and see how i can get it all to fit in the model tree.