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insert threads into hole at assembly level

17 REPLIES 17
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Message 1 of 18
SeanFarr
2619 Views, 17 Replies

insert threads into hole at assembly level

I have an assembly that is made up of 3 unique parts ( 5 parts total). These parts and there features are to be laser cut, then assembled and welded along the outer perimeter in the small chamfer. I have designed the parts to have 5/16 holes, which will be later tapped to 3/8"-16 UNC after assembly.

 

Once these parts are assembled, I don't understand how I can change the holes to reflect this. Meaning I want the parts to be pre-drilled(laser cut) with 5/16 holes, but I want the assembly to then have 3/8-16UNC holes.

 

The hole command will not let me select the existing hole features in the assembly and add threads. What is the consequence of inserting a 'new' hole with 3/8-16UNC threads over the existing 5/16" holes in the assembly?

 

Is my workflow incorrect? should I have the parts modeled with the tapped holes and just make a note on the drawing to not tap these holes until assembly? how does that affect the laser cutting?

 

Thanks

 

Sean Farr

Inventor Pro 2013

 

Sean Farr
Product Designer at TESInc.ca

Inventor Professional 2014-Update 2 - AutoCAD Electrical 2014
Win7-x64 | ASUS P8Z77-V | i7 3770 -3.4 GHz | 32GB RAM |
240GB SSD | nVidia GTX 670 4GB - 320.49
17 REPLIES 17
Message 2 of 18
SeanFarr
in reply to: SeanFarr

I can't attach .zip files that were created by windows ( right click, send to compressed .zip folder), gives me an error stating something about extension does not match binary..blah.blah.blah!!

 

 

previous post had part files, here is the assembly file,

 

any ideas of how to approach this??

 

Thanks

 

Sean Farr

Sean Farr
Product Designer at TESInc.ca

Inventor Professional 2014-Update 2 - AutoCAD Electrical 2014
Win7-x64 | ASUS P8Z77-V | i7 3770 -3.4 GHz | 32GB RAM |
240GB SSD | nVidia GTX 670 4GB - 320.49
Message 3 of 18
rdyson
in reply to: SeanFarr

IV doesn't like your 5/16 holes. The minor dia for the 3/8-16 is smaller than 5/16, so IV thinks it has no material to remove.

You might be able to edit thread.xls, don't know.

Or, change the drill size to something smaller in the ipt's.



PDSU 2016
Message 4 of 18
SeanFarr
in reply to: rdyson

So you are adding holes (threaded) over top the existing holes in the assembly? I thought there used to be an option to just thread existing holes, for a case like this? Not create new holes...

 

If I change the holes in the parts, then the drawings will be affected and the wrong sizes will be cut out. 

 

I think my best work around it to not have threads in the final assembly, their only benefit of existence that I can see (for my case) is the ease of calling them out in a drawing.

 

I have attached a drawing (not finished) of what I could probably do to bypass this issue. Edit the hole note to something like that??

 

Any other ideas are welcome, as I don't see this as solved.

 

thanks

 

Sean Farr

Sean Farr
Product Designer at TESInc.ca

Inventor Professional 2014-Update 2 - AutoCAD Electrical 2014
Win7-x64 | ASUS P8Z77-V | i7 3770 -3.4 GHz | 32GB RAM |
240GB SSD | nVidia GTX 670 4GB - 320.49
Message 5 of 18
Paul-Mason
in reply to: SeanFarr

Would it not be easier just to produce  the assembly drawing as normal then un-check the show threads option, this way you can then, from one file, produce two distinctively different assembly drawings or by the crafty use of layers settings, just as in AutoCAD, you can then switch on/off any hole/tread notes etc.

 

With the tapping hole, this seems to be an Inventor thing, I've noticed that when using some of the threads Inventor takes the tapping hole to the "nearest common available drill" even with the precision set to 1/128inch, for you r chosen thread, I can't get inventor to display below 5/16 tapping drill for this hole, when the best tapping hole will be 8mm (0.314 inch) but this can be simply worked around by editing the hole/thread text.

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Message 6 of 18
SeanFarr
in reply to: Paul-Mason

I think my last post, just before yours, is the same idea, edit the hole note to reflect the needed thread info. The hole size currently is 5/16 which the drill size for tapping 3/8-16UNC. These holes will be cut out using a laser cutter.

 

I will use an assembly drawing, the example I posted above, to ensure that the holes get tapped to once assembled. 

 

Thanks

 

Sean

Sean Farr
Product Designer at TESInc.ca

Inventor Professional 2014-Update 2 - AutoCAD Electrical 2014
Win7-x64 | ASUS P8Z77-V | i7 3770 -3.4 GHz | 32GB RAM |
240GB SSD | nVidia GTX 670 4GB - 320.49
Message 7 of 18
RobJV
in reply to: SeanFarr

I do similar work all the time.  I simply create my drawings to reflect final outcome: Example 3/8" tapped hole.  I then go into my flat pattern and edit it to show 5/16" holes instead.  This way my g-code for my plasma will be right and the final drawing is right.

 

Would that work for you?

 

Rob

Message 8 of 18
SeanFarr
in reply to: RobJV

Not sure I follow, so you create your part WITH the tapped 3/8? holes, then edit your flat pattern to show 5/16" holes?

Do you have an example?

 

I don't know how laser cutting works, whether the actual size of the hole is relevent or does the laser cutter read the parameters(dimensioning)??

 

Thanks

 

Sean

Sean Farr
Product Designer at TESInc.ca

Inventor Professional 2014-Update 2 - AutoCAD Electrical 2014
Win7-x64 | ASUS P8Z77-V | i7 3770 -3.4 GHz | 32GB RAM |
240GB SSD | nVidia GTX 670 4GB - 320.49
Message 9 of 18
hfds006
in reply to: SeanFarr

I don't like shortcuts like editing the hole note but that is a quick and simple solution I have used.

 

Another option we use with weldments is creating a derived part from the assembly. This would allow you to edit the part like any other .ipt file.

 

 

Message 10 of 18
SeanFarr
in reply to: hfds006

So using your worklfow:

  1. Create all parts ( with drill hole size and not tapped hole size)
  2. Assemble parts
  3. create a derived part from this assembly
  4. edit that derived part to reflect tapped hole size.

Some key points, the individual parts NEED to have the correct drill hole size, for production. There is an inventor issue in the assembly level, that it won't let me create a new hole over top the existing holes. If i create this derived part, will it allow me to edit those existing holes or make 3/8-16UNC holes over top of them? or will i have the same error as I do at the assembly level?

 

I am not sure if what I am doing is incorrect? the more i think about this, the more i feel it is an inventor issue.


This particular assembly requires the holes to be pre-cut by the laser cutting machine, then assembled/aligned and tapped by a worker.

 

Why can't I make this happen with inventor?

 

Thanks

 

Sean

Sean Farr
Product Designer at TESInc.ca

Inventor Professional 2014-Update 2 - AutoCAD Electrical 2014
Win7-x64 | ASUS P8Z77-V | i7 3770 -3.4 GHz | 32GB RAM |
240GB SSD | nVidia GTX 670 4GB - 320.49
Message 11 of 18
hfds006
in reply to: SeanFarr

Sean,

 

I did a quick experiment to make sure this method would work with tapping existing holes. When I use this method it is typically to do more machine work to the assembly and not tapping holes.

 

Here is the workflow I used:

1. Create individual part, with drilled holes.

2. Create an assembly from the individual parts.

3. Create a new derived part from the assembly.

4. Use the "thread" command to tap the existing holes.

 

This method worked, but not as well as I had hoped.

The problem I encountered was that the thread command would not let me select multiple holes at once.

I had to apply the thread to each individual hole, which could be very tedious if you have a large number of holes.

The biggest issue is at the drawing level. Since each hole is threaded individually dimensioning does not recognizes the holes as a group, so you still have to edit the dimension to include the proper quantity.

 

I had hoped this would be a more elegant solution. I guess this just may be another case where its difficult to recreate in Inventor what actually happens in real life.

 

Good luck,

Richard in Houston

 

 

Message 12 of 18
SeanFarr
in reply to: hfds006

OK, i'll accept this, I thought I was going crazy when I couldn't find the thread feature, but that is only available in the part level and not assembly level:

 

Well, if I am going to use this method, I will have to do another test and see if that the BOM/parts list shows the individual parts for assembly on a idw.

 

At least I can get thread to show up on the final assembly view.

 

Thanks for now!!!

 

Sean Farr

Sean Farr
Product Designer at TESInc.ca

Inventor Professional 2014-Update 2 - AutoCAD Electrical 2014
Win7-x64 | ASUS P8Z77-V | i7 3770 -3.4 GHz | 32GB RAM |
240GB SSD | nVidia GTX 670 4GB - 320.49
Message 13 of 18
SeanFarr
in reply to: SeanFarr

I don't have much experience with derived parts, but after trying to create a drawing using my example. I can't identify the unique parts that the assembly is comprised of. In the parts list I would like to show what the assembly is made up of and qty's.

 

So unfortunately, using a derived part will not be a good method for this issue.

 

The only other option I can think of is to get rid of the holes in the part level and then add the threaded holes to the assembly. If the fabricator wants to laser cut the holes before assembly, I suppose he can take the initiative and figure it out based on the hole centers off the assembly drawing, figure out what the drill size is for 3/8-16 UNC and go from there. 

 


Doesn't seem right, but at least this way, I have a drawing showing final outcome. I don't really care for this particular part how it is made.

 

Not even sure if I can make a suggestion to the idea station forum for this issue, I know why I can't add threads to the part features inside an assembly. If the part features change, then the threads at the assembly level will result in an error. Example: holes currently in parts is 5/16", which is the drill size for 3/8-16UNC. If changed the holes in the parts to 1/8", Inventor wouldn't know what to do with the 3/8-16UNC holes in the assembly level. The major issue lies with why can't I add new threaded holes in the assembly over top the existing the holes from the parts files??

 

Sean

Sean Farr
Product Designer at TESInc.ca

Inventor Professional 2014-Update 2 - AutoCAD Electrical 2014
Win7-x64 | ASUS P8Z77-V | i7 3770 -3.4 GHz | 32GB RAM |
240GB SSD | nVidia GTX 670 4GB - 320.49
Message 14 of 18
RobJV
in reply to: SeanFarr

Simply make a plate with 3/8" tapped holes.  Create a flat pattern.  Edit the flat pattern and create a sketch.  Fill in the holes.  Create a 5/16" hole with same centres.

 

The laser/plasma/oxy/water typically only uses the dxf created from the flat pattern and does not care about the model/assy.

 

Would  this not work for you?  (You can even have the holes be parameter driven.)

 

(This is another reason I would like flat patterns to be able to have the option of holes represented by points just like punches.)

 

Rob

Message 15 of 18
SeanFarr
in reply to: RobJV

Yea, sorry I did read this earlier when you wrote it and meant to reply back.

 

This just seems like alonger way around, make a flat pattern for a part that is aleady flat. I like how you can edit the parts in the flat pattern they only affect that view. Once you click back to the folded part view the editing is gone. However, this is more work than needed. I would need to create flat patterns for all three parts, ensure that I have selected the flat patterns in the individual part file drawings for annotating, and then for the assembly drawing I could have the proper final assembly with the threaded holes shown.

 

But if I keep everything as the way I have it, make the correct part files with proper drilled holes (5/16") and then in the assembly drawing, fudge the one hole note to show 3/8-16UNC, it is much less work and it gets the job done. There is no need to visually show the threads, and the part will be made accurately based on the individual part drawings.

 

I will keep this in mind though for future issues that can be resolved by this method.

 

Thanks!!

 

Sean

Sean Farr
Product Designer at TESInc.ca

Inventor Professional 2014-Update 2 - AutoCAD Electrical 2014
Win7-x64 | ASUS P8Z77-V | i7 3770 -3.4 GHz | 32GB RAM |
240GB SSD | nVidia GTX 670 4GB - 320.49
Message 16 of 18
RobJV
in reply to: SeanFarr

No problem.  Glad you found a solution that works. Smiley Happy

Message 17 of 18
IS200
in reply to: hfds006

I think the answer to this could lie within the part view representations. If we had more control over part features, then a view rep could be setup in the assembly to show either the blank holes or the threads.

I wonder if this is something Autodesk could fix by adding a Level of Detail to the part view representation tree.

Message 18 of 18
SeanFarr
in reply to: IS200

Yea, this would be another possible solutuion, maybe set up a multi-value user parameter that can changes the holes from 5/16" thru to 3/8-16UNC, and set view reps or possibly use iLogic to show thru holes in the part level and then show the tapped holes in the assembly level. Brain is churning again...

 

haha, thanks for the reply, might be onto something...

 

Sean Farr

Sean Farr
Product Designer at TESInc.ca

Inventor Professional 2014-Update 2 - AutoCAD Electrical 2014
Win7-x64 | ASUS P8Z77-V | i7 3770 -3.4 GHz | 32GB RAM |
240GB SSD | nVidia GTX 670 4GB - 320.49

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