Drawing Multiple Angled Holes In bock

[DanMcManus2492]

I need to create a adaptor to go from one 96 hole array pattern to a smaller 96 hole array pattern.  The pattern gets smaller in both X and Y.  This would go from vertical hole to angled hole back to vertical hole.  One or both of the vertical sections could be removable to allow this to be a drilled part.  The center section would be a solid block. 

Since each hole will be at a different angle (in two different planes) it seems like I would need to create a seperate plane for each hole and extrude from that plane.  In addition to being error prone, this would take a large amount of time.  Is there an easier way? 

It would be straight forward to create a block with points for the large 96 hole array on top and the small 96 hole array on the bottom.  Is there some kind of point to point method of creating a hole at an angle?  A construction line could be drawn point to point but is there a way to make a hole from that?

[SBix26]

Symmetry will be helpful here, so you will only need to model one quarter of the holes and then mirror the rest.  And yes, you can construct work axes point to point. Holes can be placed using a point (work point) and direction, so this may be all you need.  But that's still 24 separate work axes, work points, and hole features.  There must be an easier way, but I don't have time to play with it now.

In case anyone else does, please tell us what version of Inventor you're using, and the array layout-- 12 x 8? 16 x 6? 24 x 4?

Sam B
Inventor 2012 Certified Professional

Please click "Accept as Solution" if this response answers your question.
-------------------------------------------------------------------------------------
Inventor Professional 2013 SP1.1 Update 2
Windows 7 Enterprise 64-bit, SP1
HP EliteBook 8770w; 8 GB RAM; Core™ i7-3720QM 2.60 GHz; Quadro K4000M
SpaceExplorer/SpaceNavigator NB, driver 3.16.2
still waiting for a foreshortened radius dimensioning tool in Drawing Manager

[VdVeek]

Dan, You didn't tell which Inventor version you where using. I hope you use 2013 so you can open my attached file, because it's a bit difficult to tell. But you can do it by creating one side of the rectangle, create workplanes and work axises and 1 extrude hole. Now circular pattern this hole over the angled workplane. Hope that it make sense to you when you open my file. (In the part the driven angle is changed after creation to 147,94 but it's value is wright 32.06)

Rob.

[swhite]

If your hole size stays the same you can use the Sweep feature with the holes and a line for the path. You could also use the Loft feature, but sweep is prefered duo to simplicity and file size. Draw a line between holes at the path you want the hole to follow and select sweep and use the hole as the profile and the line as the path.

Will give you something similar (simple example:

[DanMcManus2492]

I'm running version 10.  We have 13 but activating licenses has been a real nightmare for us.  Some pics of the tube version are attached.  This has one straight hole and the others at increased angles but the patterns could be centered to allow your "mirror 24" recommendation.

The angled holes will not be perpendicular to the start or end surfaces.  Would those other functions work?

Thanks

[JDMather]

Let me see if I understand the design intent.

You want to replace those tubes with a solid part with holes where those tubes are now. Correct?

Will the tubes be completely replaced by the solid or run in the holes in the solid?

I'm going to suggest an unconventional technique using Routed Systems electrical wire routing (assign pin numbers on each of the plates that then sweep a circle (Route) between them).  Then Derive Component to cut the channels, but the question that remains is, "How will this be manufactured?"

[graemev]

This may be what you're looking for.  I've labeled the construction geometry for the first two rows so you can (hopefully) follow what I was doing.  The third and fourth rows follow the same work flow.  You can fiddle with the user parameters to change the X- and Y-spacing, as well as the X- and Y-hole counts.  The block's overall dimensions are right at the top in the parameter list, and the hole diameter and depth are d70 and d71 respectively.

Modelled in IV2013.

P.S.  Your production department will despise you when they find out about having to do 48 individual setups. 

[SBix26]

Rob, assuming that the 12 x 8 array is evenly spaced on both top and bottom plates, your polar array won't work, because the spacing isn't even.  I still haven't come up with any other method than a lot of hard work, but I've never used the wire routing functionality that JDMather is proposing-- hopefully Dan has Inventor Professional and that will work for him.

Dan, be careful with version numbers.  It sounds as if you might be using Inventor 2010, which is four years newer than Inventor 10, released in 2005 (?).  Inventor 2010 is actually version 14.

Graemev, a five-axis mill should be able to do the drilling without anybody breaking a sweat...

Sam B
Inventor 2012 Certified Professional

Please click "Accept as Solution" if this response answers your question.
-------------------------------------------------------------------------------------
Inventor Professional 2013 SP1.1 Update 2
Windows 7 Enterprise 64-bit, SP1
HP EliteBook 8770w; 8 GB RAM; Core™ i7-3720QM 2.60 GHz; Quadro K4000M
SpaceExplorer/SpaceNavigator NB, driver 3.16.2
still waiting for a foreshortened radius dimensioning tool in Drawing Manager

[VdVeek]

Dan, That's a shame you haven't 2012 or 2013. But i made some screenshots of the steps you can follow.

This is only the plate with the holes under an angle. The top and bottom plate are just straight forward.

Step.1 Create the part shape and place a sketch on the topside with an rectangle the size of the large array. And on the bottomside a sketch with an rectangle the size of the small array. 

Step2. Create a workplane with 'Two Coplanar Edges' and select one line of the top sketch and the other of the bottomsketch of the same side.

Step.3 Place a sketch on the new workplane and draw 2 lines from the top corners to the bottom corners and let them intersect. Place an angle dimension between them for later use in the circular pattern.

Step.4 Place a work Axis with the option: 'Normal to Axis throug point' on the workplane and the intersection of the 2 lines is the point to click.

Next steps in next post.

Rob.

[VdVeek · Accepted solution]

Step.5 Place a workplane at the bottom end of the intersecting line and create a sketch on it with the 'hole' to extrude.

Step.6 Extrude the sketch to cut the part and give it a distance well after the topside of the part, otherwise it won't pattern right.

Step.7 Circular Pattern the hole around the rotation_Axis and use the angle dimension. Now you have one row of holes. Create an other Rotation axis for the other direction and do again a circular Pattern for the other side by selecting the side pattern. 

I hope it's a good option for you.

Rob.

[JDMather]

ah, now that I see Rob's depiction the problem is easier than I was proposing.

I was thinking like a header where the holes were curved pretty much the same as those plastic tubes.

But back to my Routed Systems idea, the wire routing allows straight line or "Natural" (curved - perpendicular at set distance to planar face pin location), so defining pins (pattern) and autorouting might still be an easy solution.  (haven't tried it yet, waiting for confirmation on design intent)  Intersting enough problem for a clever work-around that I might try it anyhow.

[graemev]

VdVeek - Pretty much exactly like the one I uploaded, the difference being that the second circular pattern creates an "hourglass" grouping of centers on the top and bottom faces of the block.  My version doesn't have that, but requires doing each row for half of the block, then mirroring the lot.  Work flow for each row is the same.  It's a bit more tedious, but the result is rectilinear.

[swhite]

Just did one hole, but something similar?

[DanMcManus2492]

The version I have is 2010 but I do not have routed systems.  The tubes would go away and be replaced with simple holes in a block.  Thanks for all of this.  I need to spend some time giving it a try.

[DanMcManus2492]

Rob,

Excellent solution....Thanks

[SBix26]

Just be sure that you're OK with the holes not being evenly spaced.  This is a much easier solution to the problem than creating an axis for each hole, but if your top and bottom plates have evenly spaced holes, you don't have much choice.

With Rob's very elegant solution, the transition plate determines the hole locations on the top and bottom plates, which have to be individually marked in the sketch, but can be placed as one hole feature.

Sam B
Inventor 2012 Certified Professional

Please click "Accept as Solution" if this response answers your question.
-------------------------------------------------------------------------------------
Inventor Professional 2013 SP1.1 Update 2
Windows 7 Enterprise 64-bit, SP1
HP EliteBook 8770w; 8 GB RAM; Core™ i7-3720QM 2.60 GHz; Quadro K4000M
SpaceExplorer/SpaceNavigator NB, driver 3.16.2
still waiting for a foreshortened radius dimensioning tool in Drawing Manager

[VdVeek]

@Dan, I see you got it working.

@Sam, you're right about the uneven spacing, hope that it's no issue for Dan. 

Rob

[DanMcManus2492]

Can you define what you mean by not evenly spaced?  It just needs to mate the two hole patterns top and bottom.  The angles holes come out a bit oval when they break the surface so actually increase in size a bit. This is for low speed fluid flow so a perfect match is not needed. 

[SBix26]

Merely that the distances between hole centers is not equal.  The mating blocks will not be able to use an array of holes, because they won't match.  They'll just have to use projected hole centers.

Sam B
Inventor 2012 Certified Professional

Please click "Accept as Solution" if this response answers your question.
-------------------------------------------------------------------------------------
Inventor Professional 2013 SP1.1 Update 2
Windows 7 Enterprise 64-bit, SP1
HP EliteBook 8770w; 8 GB RAM; Core™ i7-3720QM 2.60 GHz; Quadro K4000M
SpaceExplorer/SpaceNavigator NB, driver 3.16.2
still waiting for a foreshortened radius dimensioning tool in Drawing Manager

[graemev]

VdVeek's solution will not result in a match to the front and rear plates' hole patterns.

Try this:  (Done in IV2013)

User parameters:

How they're used:

Front hole locations - first and last in each row get a construction point:

Rear hole locations - likewise:

Two axes through first and last hole centers, front and rear, and a work point at their intersection:

A plane of two axes and a sketch dimensioning the angle between the axes (projected onto the plane):

An axis perpendicular to the previous plane through the workpoint (future circular pattern axis), a workplane perpendicular to one of the hole axes through the same workpoint, and a circle of desired hole size extrude-cut through:   (I did as an overly long distance extrude - to face didn't seem to want to array correctly, nor did a conventional hole.)

Circular pattern using the extrusion and aforementioned axis:

Same work procedure - Row 2:

All rows:

And mirror for the final part:

You will notice that the circular pattern results in unequal hole spacing whereas the individual planes result in perfectly equal spacing.  For a proper grid match you will need to do individual axes for each hole, I suspect.