Trying to Loft a hook

[Red_Stafford]

Hi all I am trying to draw a hook but I am getting problems when using the LOFT command, I get the following error "MODELING FAILURE: A RAIL CURVE INTERSECTS A SECTION MORE THAN ONCE"

See my attached drawing

[JD Mather]

Go through these tutorials - especially MA13 and MA 105 http://home.pct.edu/~jmather/content/DSG322/inventor_surface_tutorials.htm

Your sketches are unconstrained and the rail connection points not projected to the cross-section profiles. You are doing way to much work with far far too many dimensions. Start using sketch constraints like = to replace duplicate dimensions. (Let me guess - you brought this in from AutoCAD and used the Autodimension?)

Use the origin and BORN techniques as described in the linked documents.

[Red_Stafford]

Go through these tutorials - especially MA13 and MA 105 http://home.pct.edu/~jmather/content/DSG322/inventor_surface_tutorials.htm (http://home.pct.edu/%7Ejmather/content/DSG322/inventor_surface_tutorials.htm)

Your sketches are unconstrained and the rail connection points not projected to the cross-section profiles. You are doing way to much work with far far too many dimensions. Start using sketch constraints like = to replace duplicate dimensions. (Let me guess - you brought this in from AutoCAD and used the Autodimension?)

Use the origin and BORN techniques as described in the linked documents.

Cheers, this was not imported from AutoCAD but I do have a AUtoCAD back ground, it was all done using Inventor 2008 but I did use auto dimension, you post kind of lost me but I will have a ready through that site.

[JD Mather]

you post kind of lost me...

When you read those documents you will see that I suggest sketching one line, arc or polygon and dimension it immediately. Then as you add additional geometry dimension (preferably use sketch constraints like tangent, horizontal, vertical, coincident, colinear...) as you go.
When geometry is fully defined it will turn color.
Notice that my sketch (see attached) is much cleaner than yours and I needed far fewer dimensions.

I never ever use Autodimension.

Until you understand the techniques for building robust, fully constrained sketches I would work on easier parts than this one. Loft is an advanced function.

[Red_Stafford]

When you read those documents you will see that I suggest sketching one line, arc or polygon and dimension it immediately. Then as you add additional geometry dimension (preferably use sketch constraints like tangent, horizontal, vertical, coincident, colinear...) as you go.
When geometry is fully defined it will turn color.
Notice that my sketch (see attached) is much cleaner than yours and I needed far fewer dimensions.

I never ever use Autodimension.

Until you understand the techniques for building robust, fully constrained sketches I would work on easier parts than this one. Loft is an advanced function.

The thing is I need to draw this for work, I have deleted all my dimensions and added the ones you have on your pic and it says i need 29 dimensions ?

[Aardvark]

Use constraints. If you don't know what those are, read JD's tutorials and look it up in the help.

Then, I would practice on some simpler designs until you get the basic concepts down, and then try to tackle the loft.

Finally, when this project is finished, I would write an email or have a sit down discussion with your boss about getting some Inventor training. AutoCAD is not Inventor and vice versa.

Remember these words, "Forget everything you know about AutoCAD."

[Red_Stafford]

Use constraints. If you don't know what those are, read JD's tutorials and look it up in the help.

Then, I would practice on some simpler designs until you get the basic concepts down, and then try to tackle the loft.

Finally, when this project is finished, I would write an email or have a sit down discussion with your boss about getting some Inventor training. AutoCAD is not Inventor and vice versa.

Remember these words, "Forget everything you know about AutoCAD."
I am doing a part time course but for know I need to get this hook sorted so all I can do is keep trying with your help

[JD Mather]

...it says i need 29 dimensions ?

You must have missed the suggestion in the paper that says to sketch one entity and dimension/constrain immediately.

Here are the steps I would use

#1 Start over from scratch. (you can use the original for reference)
#2 Sketch arc and dimension constrain. look in lower right corner of screen if it says it needs any dimensions/constraints then attach the file here.
#3 Sketch next entity and repeat Step #2 as far as constraining/dimensioning and attaching here.
Entity by entity we can solve this problem, and yes, it will be faster to start over.

[shift1313]

what were you given by your boss to draw this hook? Do you have a certain spec? Is this going to be produced?

[Red_Stafford]

what were you given by your boss to draw this hook? Do you have a certain spec? Is this going to be produced?

It for a colleague to take to one of our supppiers to see if they can supply something simillar this is just part of it I have drawn the rest no probs it's a pully and that hook goes on top

[Red_Stafford]

When you read those documents you will see that I suggest sketching one line, arc or polygon and dimension it immediately. Then as you add additional geometry dimension (preferably use sketch constraints like tangent, horizontal, vertical, coincident, colinear...) as you go.
When geometry is fully defined it will turn color.
Notice that my sketch (see attached) is much cleaner than yours and I needed far fewer dimensions.

I never ever use Autodimension.

Until you understand the techniques for building robust, fully constrained sketches I would work on easier parts than this one. Loft is an advanced function.

How did you create your sketch did you do it using three point arcs around each of the lines coming from the centre like I have ? yours looks neater than mine and you dont even have anything in front of you to draw it from.

[Red_Stafford]

ok I think I give up, I have been trying to do this hook since last week and I have not got a clue.

[shift1313]

Red, the issue is you jumped into the deep end, you may be able to paddle around but you just dont have enough training to move around smoothly.

If you sit down and go through some of JDs tutorials he linked to I think it will all make a lot of sense. Once you get a feel for the proper way to dimension something and how to use constraints you will be much better off with trying to model this.

My copy of inventor at home hasnt worked for some time so unfortunately I cant help you out from here.

[JD Mather]

ok I think I give up, I have been trying to do this hook since last week and I have not got a clue.

Why would you give up when I offered to walk you through this literally step-by-step?

Sketch a circle - attach the file.

[Red_Stafford]

Why would you give up when I offered to walk you through this literally step-by-step?

Sketch a circle - attach the file.

Sorry dude just getting fustrated, ok I have sketched and dimensioned a circle see attached.

[Red_Stafford]

Ok I have sketched the hook out again it as also all turned colour to say its contrained but I am still having problems trying to use loft, see below link to file.

http://www.mediafire.com/?sharekey=dff5ca03dffd1b6d391d7d881749d3a7e04e75f6 e8ebb871

[JD Mather]

I have sketched and dimensioned a circle see attached.

I do not see any evidence that you read the documents I suggested earlier.

Pay particular attention to http://home.pct.edu/~jmather/AU2007/MA105-1L%20Mather.pdf
Tip #8 to turn on the visibility of the origin and Project Geometry the origin Center Point. You want this to be at a logical location in the part.

There is no point in continuing until that basic principal is understood. Out on the shop floor the first thing the mill or lathe operator does in setting up a job is determine 0,0 location.

I looked at your hook 4 - I never ever use Fixed constraint - use the origin. Also you need to use many many more tangent contstraints where appropriate and also = constraints. If you see dimensions repeating over and over again (like for fillets) there should be only one dimension with the rest replaced with = constraints.

[Red_Stafford]

Ok, see attached circle I have turned the center point on.

[JD Mather]

Nope

See Tip #4 to Autoproject part origin on sketch create

and tip #10 for green "hard snap" placing coincindent constraint.

If you do not see this green dot then you need to Project Geometry the origin Center point yourself (rather than relying on automatic as decribed in #4. Project Geometry will be one of the most important concepts in creating the section profiles for this hook.

If you can drag your circle it isn't anchored. It didn't change color - so it isn't constrained.

Think of it like dropping a block of aluminum on the milling machine table and trying to make a cut. If you don't anchor it down all kinds of bad stuff is going to happen. No machinist could ever get away with work like this.

Of course because we are doing this step-by-step over the internet it will be far more frustrating and far less efficient than classroom training.

JD
Certified Machinist

[Red_Stafford]

Nope

See Tip #4 to Autoproject part origin on sketch create

and tip #10 for green "hard snap" placing coincindent constraint.

If you do not see this green dot then you need to Project Geometry the origin Center point yourself (rather than relying on automatic as decribed in #4. Project Geometry will be one of the most important concepts in creating the section profiles for this hook.

If you can drag your circle it isn't anchored. It didn't change color - so it isn't constrained.

Think of it like dropping a block of aluminum on the milling machine table and trying to make a cut. If you don't anchor it down all kinds of bad stuff is going to happen. No machinist could ever get away with work like this.

Of course because we are doing this step-by-step over the internet it will be far more frustrating and far less efficient than classroom training.

JD
Certified Machinist

Ok cheers I have projected the centre point, see attached.

How do I get into the options screen that you have on your tutorial ?

[JD Mather]

How do I get into the options screen that you have on your tutorial ?

Tools>Application Options

[Red_Stafford]

Ok this is where I have got to so far (see attached) but it is still not right ?

http://www.mediafire.com/?sharekey=dff5ca03dffd1b6d391d7d881749d3a7e04e75f6 e8ebb871

[JD Mather]

Ok this is where I have got to so far (see attached) but it is still not right ?


I don't normally go to sites like that to download stuff. If you drag the red End of Part marker in the feature tree to all the way to the top before saving and zipping that usually makes a file small enough to attach here.
Then on my end I simply drag the EOP back down.

[JD Mather]

I backed up a bit on your sketch.

There is no Horizontal constraint on the 56mm line which is obviously intented to be horizontal. Add the constraint.

These outside arcs all need to be Tangent to create a smooth part - add Tangent constraints.

The 46mm line does not go through the centerpoint as it should.

These radial lines aren't part of the rail, so they should be Construction linetype (see attached).

I would replace the Ø30 dimension with a R15 dimension (you can even do this before it was trimmed when it was still a circle by right clicking when placing the dimension.

With this part Tangent is your friend.

In the attached I demonstrated pulling up the EOP to make the file size as small as possible, simply drag it back down below Sketch1.

[Red_Stafford]

I backed up a bit on your sketch.

There is no Horizontal constraint on the 56mm line which is obviously intented to be horizontal. Add the constraint.

These outside arcs all need to be Tangent to create a smooth part - add Tangent constraints.

The 46mm line does not go through the centerpoint as it should.

These radial lines aren't part of the rail, so they should be Construction linetype (see attached).

I would replace the Ø30 dimension with a R15 dimension (you can even do this before it was trimmed when it was still a circle by right clicking when placing the dimension.

With this part Tangent is your friend.

In the attached I demonstrated pulling up the EOP to make the file size as small as possible, simply drag it back down below Sketch1.

Ok cheers but I cant open the file as I am using Inventor Prof 2008

I have made some of the mentioned amendments, what do you think, its not all changed colour ?

[JD Mather]

You were still missing a few dimensions - but I think you have to admit - you've made a lot of progress since that rat's nest you had yesterday.

You still have a bit of work to do on the section profiles - Tip: same number of entities in each connecting profile will make your life easier.

Change those lines to Construction linetype (toggled in upper right corner of screen while in sketch mode).

[Red_Stafford]

Cheers JD, see attached file this is where I am at the moment but still strugling to loft.

[JD Mather]

The transistion at the base of the hook is too sharp. In fact, following the rail it curves back over itself (see attached).

Probably need to move that circle down to where the horizontal line passes through the R5 curve.

The add another section circle at 45°. You will have to use a series of Lofts - I don't think you can get this all with one loft.

[Red_Stafford]

The transistion at the base of the hook is too sharp. In fact, following the rail it curves back over itself (see attached).

Probably need to move that circle down to where the horizontal line passes through the R5 curve.

The add another section circle at 45°. You will have to use a series of Lofts - I don't think you can get this all with one loft.

Ok I think I have corrected that but the loft still doesnt work, see attached

[Red_Stafford]

Can any else give me a hand with this, I have got till tomorrow to sort this hook out ?


Prety please...

[shift1313]

sorry red i cant open your files because im using an older version.

have you dont any simple lofts and had them work? Have you gone through the tutorials JD posted?

[Red_Stafford]

sorry red i cant open your files because im using an older version.

have you dont any simple lofts and had them work? Have you gone through the tutorials JD posted?

I have read the tuturials and I have also managed to loft other things.

[shift1313]

where is the issue with this one at?

[JD Mather]

I have read the tuturials and I have also managed to loft other things.

I noticed that you had a bunch of extra projected stuff in each of the profile sketches and that at least one was not attached to the rails.

I normally check this as I go along.
Create the first two profiles.
Try to loft with rails. OK then undo.
Sketch next profile.
Try again. OK undo.
Not OK figure out why.

Once you do these steps you start to learn how to create clean connected sketches.

I added the angled circle sketch to replace the flat circle sketch you had near the base and another angled sketch near the hook.

I didn't take the time to find the missing connection to the rail -which results in the bumb discontinuity seen in attached image.

Do you have a picture of the actual part?

[Red_Stafford]

So you suggest deleting the sketches and do them again one by trying each one at a time.

See attached pic.

[shift1313]

if you have rails you dont need to select all your profiles. I dont know that i would delete everything

[JD Mather]

So you suggest deleting the sketches and do them again one by trying each one at a time.

See attached pic.

Well, actually I simply started over using what was learned from the first couple of attempts and your pics. About 6 hours of work this is what I came up with. I will explain the steps over the next few days as I find time. Suffice to say this is not a beginner project, although I will make it look fairly easy.

[JD Mather]

First of all I simplified the main loft feature as the beginning and end sections (and all intermediate sections) were identical except for the height.
By projecting the rails 14/2 and 25/2 on either side I needed only the two end profiles.

[Red_Stafford]

Well, actually I simply started over using what was learned from the first couple of attempts and your pics. About 6 hours of work this is what I came up with. I will explain the steps over the next few days as I find time. Suffice to say this is not a beginner project, although I will make it look fairly easy.

That is quality.

[JD Mather]

When examining your sketches I realized the last two on the end of the part were same size rectangles. This means that geometry could be created with a simple Extrude feature rather than a Loft. At the beginning end I Lofted the circles.

[JD Mather]

Then I lofted the main center section using all of the rails.

[JD Mather]

Then I blended the end to the middle section using Loft with G2 smooth tangency. Keep in mind to select the center rails you have to pick twice - once to select the sketch and a second time to select the rail.
Finally, I added Variable Radius Fillets to the hook edges. This takes a lot of experimentation and prior knowledge to get them to work out.

Now that you understand the geometry doing different itterations takes much less time.

[JD Mather]

I should have pointed out - when doing blending fillets like shown in the previous post - select the faces of the part rather than sketches for the section profiles or you won't get the option for G2 tangency.

[lis_wang]

How to create this hook in the attached file?

Would you like to email the hook you created to me?

[JD Mather]

Attach what you have completed so far.

[lis_wang]

The attachment is the hook I created. I do not know how to make the sharp corner to sphere R6.

[lis_wang]

The attachment is the hook I created. I do not know how to make the sharp corner to sphere R6.

I have amended the hook. Please take a look.

[JD Mather]

This could be simplified a bit more as a couple of the sketches aren't really needed. The Workpoints aren't really needed. Well looks like I will have to simplify as it won't quite fit here because of filesize. Just realized I had the Spherical Radius as 2 rather than as 6 like print dimension. I will post corrected attachment when I get it under 250K.

[JD Mather]

I made a mistake causing to have to do the Loft as a surface and then Sculpt to get solid (bit tricky to explain the mistake). So the Sculpt is an extra step, but you should get the idea.
To reduce file size I omitted the cylinder, chamfer and thread.

[lis_wang]

I made a mistake causing to have to do the Loft as a surface and then Sculpt to get solid (bit tricky to explain the mistake). So the Sculpt is an extra step, but you should get the idea.
To reduce file size I omitted the cylinder, chamfer and thread.

I have not problem to create loft for your "sculpt1" as solid output. But I cannot create the loft as your Loft 1. My problem is I cannot select the outer portion of sketch 1 (the arcs of R70 and R82) as Rails. How did you manage to select sketch 1 twice as rails?

[linnmaster]

I have not problem to create loft for your "sculpt1" as solid output. But I cannot create the loft as your Loft 1. My problem is I cannot select the outer portion of sketch 1 (the arcs of R70 and R82) as Rails. How did you manage to select sketch 1 twice as rails?

HI ...
When you pick the the rails ... you have to select each rail twice. You'll see when you pick one rail, on the very bottom of the screen in the message bar, it says something along the lines "sketch contains more than one open loop, and you need to pick one".
So, when you select your first rail ... select the inside curve, it will only highlight partial ... place your cursor over the same rail again, and it will highlight the entire curve up to the radiused end.
Add new sketch, and do the same with the outside curve ...

Should work ...

[linnmaster]

My question is why can't the first loft be created as solid? It seems to fail and only works with surface ...

And the other question is that for Loft1, you've got both tangent conditions on both edges that are selected ... When I tried tangent on both, it turns really ugly ... only on the edge at the tip radius 6 end it becomes more like "normal" when the "tangent" condition is selected ... the other end is fine and works with tangent, like it should. Any idea why the different results between the two?

[shift1313]

My question is why can't the first loft be created as solid? It seems to fail and only works with surface ...

And the other question is that for Loft1, you've got both tangent conditions on both edges that are selected ... When I tried tangent on both, it turns really ugly ... only on the edge at the tip radius 6 end it becomes more like "normal" when the "tangent" condition is selected ... the other end is fine and works with tangent, like it should. Any idea why the different results between the two?


which hook are you speaking of? JD used Smooth(G2) tangency. It will produce a different result than tangent.

[JD Mather]

My question is why can't the first loft be created as solid? It seems to fail and only works with surface ...

If you test the closed sketches in my previous model by trying to Extrude you will see a red cross in the dialog box. This is associated with coincident points that did not merge. (Tip: Doing Extrude even when my end design intent is not an extruded feature is the easy way that I test closed sketches for this problem.)
In Rev2 I have fixed things up.



When I tried tangent on both, it turns really ugly ... only on the edge at the tip

Attach your file here. In my file you should notice that the tip is only part of the spherical feature (not a hemi-sphere).

[linnmaster]

I can't seem to get my file small enough - I'm out by 8kb ... here is a screen shot of what happens on the final loft3 when both edge conditions are set with tangency condition ...

Anyways, I just recreated the features that JD did on his (or tried to), using his sketches ... and it seems like my end result is different ...

http://img411.imageshack.us/img411/2093/hookdl.jpg

[linnmaster]

I just realised something ... I seem to have two solid bodies ... and I think this is creating my problems seen above ...

Nope ... got it as one solid, but symptoms are still the same as above with tangency condition set on both edges on final loft ...

[linnmaster]

If you test the closed sketches in my previous model by trying to Extrude you will see a red cross in the dialog box. This is associated with coincident points that did not merge. (Tip: Doing Extrude even when my end design intent is not an extruded feature is the easy way that I test closed sketches for this problem.)

JD. Not sure quite what you mean as all your closed loop skteches do Extrude. However, there is a red cross in the dialogue box that shows up, but, it's for the sketch that contains the rails ... which is of course open.

[linnmaster]

which hook are you speaking of? JD used Smooth(G2) tangency. It will produce a different result than tangent.

In JD's model, he didn't use Smooth(G2). He used Tangent. When I use Tangent, I get what you see in my screen shot above. To get something similar to JD's rev1 model, I had to use Free. Using Smooth(G2) becomes too fat.

Regards,
David

[JD Mather]

JD. Not sure quite what you mean as all your closed loop skteches do Extrude. However, there is a red cross in the dialogue box that shows up, but, it's for the sketch that contains the rails ... which is of course open.


I didn't say they won't extrude (the closed profiles, not the rails sketch). I said in the original example I posted if I try to extrude as a test of the quality of the closed profile sketch there is a red cross (they will still extrude).

In the second example if you try to extrude (the closed profiles) as a test there is no red cross.

[JD Mather]

...here is a screen shot of what happens on the final loft3

Did you take a look at the Rev2 file I posted? You need to be careful where you select the edges for the loft. Click on the planar faces near the edge or the tangency will be to incorrect face.

Note also that must have existing solid faces or surfaces to get the tangent options. Lofts with sketches do not give this option.

[linnmaster]

In the second example if you try to extrude (the closed profiles) as a test there is no red cross.

I still see a red cross. Click on the red cross, and it runs through it's diagnosis and picks up the open profile on the sketch that contains the rails ....

Hence I can't really see any difference between rev1 and rev2, except one works with loft as solid, and the other needs to be lofted surface first, then sculpted.

[linnmaster]

Did you take a look at the Rev2 file I posted? You need to be careful where you select the edges for the loft. Click on the planar faces near the edge or the tangency will be to incorrect face.

Note also that must have existing solid faces or surfaces to get the tangent options. Lofts with sketches do not give this option.

Ahhh! I see! Thanks so much for the clarification and pointing to where the issue might be.

Oh, and yes, I looked at Rev2.

Regards, David

[JD Mather]

I still see a red cross. Click on the red cross, and it runs through it's diagnosis and picks up the open profile on the sketch that contains the rails ....


Not the rail sketch - that one is open and therefore should have a red cross.

[lis_wang]

Not the rail sketch - that one is open and therefore should have a red cross.

Your Rev2 file has a minal mistake, the dimension 38 for sketch 3 is from side to side, instead of from center to center.

Thank you very much JD.

[Safwah]

Hey JD are you just using inventor for those renders on page 4 of the hook? They look very sharp, id like to get my renders to that quality. Can you attach the finished file for that so i can take a look at the rendering options/settings. Thanks

[linnmaster]

Hey JD are you just using inventor for those renders on page 4 of the hook? They look very sharp, id like to get my renders to that quality. Can you attach the finished file for that so i can take a look at the rendering options/settings. Thanks

I had a look earlier, and it seems to be just material settings ... select the surface, right click, options, material ... for the the matt hook finish - it's cast aluminium ... for the shiny thread part ... polished alumnium? Hope that helps. Regards, David

[Safwah]

I had a look earlier, and it seems to be just material settings ... select the surface, right click, options, material ... for the the matt hook finish - it's cast aluminium ... for the shiny thread part ... polished alumnium? Hope that helps. Regards, David

What about the background, just a custom background image? Seems to make sense now. Now why cant we render that well with inventor :P Meh practice i suppose.

[linnmaster]

What about the background, just a custom background image? Seems to make sense now. Now why cant we render that well with inventor :P Meh practice i suppose.

Heya ... I never took much notice of the background - are you talking about way earlier with the faint grid? If you are, then wait for JD's response.

I personally can't be bothered with the background, or the appearance of the model, because for me, at the end of the day, the drawing is what's important, and (btw, I learned this the hard way) after many nights without sleep spent trying to model it perfectly, and get it all looking nice, you STILL HAVE THE DRAWING TO DO!!! If you have time, it's great fun and good learning to make the model look like JD's, and it's great for presentation purposes, but in my world, people couldn't care less ... the drawing is the key ... so keep that in mind :)

Just my opinion and my experience ....

[Safwah]

Oh yeah, dont get me wrong, im up the with the better users when it comes to inventor and the drawing comes first as you say, although in my free time i try to master the program by working on areas like rendering in inventor, it has its uses as some clients have requested presentation drawings but i can just never get it to look sharp in inventor. Id say the faint grid is just a custom background being used.

Eg. I know i can do better then this, just cant seem to get the quality im after in inventor though.

[linnmaster]

OMG! That's freaking awesome! Now if only I can do that lol ... :)

[Safwah]

Maybe its a matter of looking at the same thing all day i only notice the problems rather then standing back and saying "look what i have created!" :P

[JD Mather]

i can just never get it to look sharp in inventor. Id say the faint grid is just a custom background being used.

The grid was not a custom background - one of the standard backgrounds in Inventor Tools>Application Options>Colors tab.

Search Google for Bill Bogan Inventor Studio Tutorials.

Also Mark Flaylor has several here http://au.autodesk.com
look in the Online classes.

[Safwah]

Nice thanks JD, ill take a look at those tuts. Hard to come by some decent tuts on studio, most are just "so this is how you get into studio, use the presets, done bleh."

[john7911]

Thank you i'll try to do this hook for practis

[lis_wang]

I cannot do the loft portion for the frame. The trail looks like a 3D sketch. Please see what I have done.

[JD Mather]

Everyone else - give it an honest try before you look at my example.

Just realized I made a slight mistake - change the 38 dimension in Sketch1 to 44. Change Thicken1 to 44 as well.

I realized that I didn't need the second extrude surface and be very very careful with ribs. Keep in mind that when we drew in 2D that rib extents are simplified. In 3D we have to be a bit more true to the real geometry.

[lis_wang]

Everyone else - give it an honest try before you look at my example.

Just realized I made a slight mistake - change the 38 dimension in Sketch1 to 44. Change Thicken1 to 44 as well.

I realized that I didn't need the second extrude surface and be very very careful with ribs. Keep in mind that when we drew in 2D that rib extents are simplified. In 3D we have to be a bit more true to the real geometry.

Dear JD

Your method is excellent. I tried to use LOFT with 3D sketch trails. It looks very bad.

[arshavin23]

Good work JD!

[pinco pallino]

I cannot do the loft portion for the frame. The trail looks like a 3D sketch. Please see what I have done.

Hi Lis
if that fork is to be cast in sand or forged
those concentric ribs around the big hole are making an under cut
that's a trouble for pattern making and it will cost big dollars to produce
consider make them perpendicular to the the join line (larger surface).
Regards Ralf
engineering pattern-maker designer

[lis_wang]

Hi Lis
if that fork is to be cast in sand or forged
those concentric ribs around the big hole are making an under cut
that's a trouble for pattern making and it will cost big dollars to produce
consider make them perpendicular to the the join line (larger surface).
Regards Ralf
engineering pattern-maker designer


What do you mean by " perpendicular to the the join line "?

Thanks

[JD Mather]

I assumed this was merely an academic excersize and not that you are going to actually manufacture. If you are going to manufacture you should establish parting line for the mold and run Draft Analysis. Make sure all of your faces have appropriate draft.

I normally do a Derived Component and remove Holes and add material for machining to faces that will be machined as well for the As Cast model.

[pinco pallino]

What do you mean by " perpendicular to the the join line "?

Thanks

JD is right, this is only a practice exercise to master the use of inventor.
And my point is out of topic. Sorry about that. I reply just to bring a conclusion to the mess I started.
The rib here is perpendicular to the join line.
For moulding purposes the pattern will be made spit in 2
The split is the join line. The taper and machining allowance is a pattern-maker's concern, you don't have to draw them, a tolerance shown on the faces to be machine is all it needs.