This has been in my drafts way to long. I only allowed myself to publish new posts if there is one ready to go in my drafts. Even though I am not back to normal I feel this might help me move towards normality even if I might never get there again. Can fittings have both male/female connections and different
engagement distance?
My friend asking this was referring to elements like bushings, and
reducers as in the image bellow where the right side connection can fit 2
sizes, one inside (female) and one outside (male). These will need different
engagement distances as well.
3 connections on same fitting.
Library or stand alone?
There is no gender on the fittings; they are all connected by
points and axes but how you author it depends on what you intend to do with the
file. Is this for an ipart to be published to Content Center, or is it a
standalone library file?
More than likely this will be used in content center but if this
is a standalone library then you need to author this in a weird way with 3
connections instead of 2. When you place the fitting press Spacebar until it
shows the correct position.
While this is possible I think most of you will need this in
Content Center. For that you will create two identical shape members with
different connections.
Even though these members will have identical part number, stock
number and whatever fields you use to identify this, the filename needs to be
unique. This is one rare occasion when I allow filename to be different than
the part number.
How do we create a dynamic engagement distance? You create an
offset work plane and you control the offset value from the ipart table.
offset plane
ipart table
In the author fitting window choose Engagement, To Plane, Point
and choose our plane.
This is last
part of the series, covering how to publish dumb parts to Content Center. Now
you know where to get
parts on the internet, how to create work features,
and how to author
empty parts. This is all neded info before we take the final step.
Quite
simply publishing dumb parts as a family in content center is based on the
ability to create iparts with suppressed bodies (will expand later).
Downloaded parts can stay dumb, we'll make them smart.
As
you probably know if you follow this blog when I download parts from the
internet I don’t publish them to content center but I keep them in a library
folder and the document properties are saved in a text file. When I need to
place a certain valve I copy the file path from the text document, and I paste it in the place fitting dialog window to speed up my navigation time.
Content center seems slow as it is and I don't want to overload it with
individual parts.
While
placing from disk is faster than placing from content center (it is for me)
there is another limitation that we can’t overcome. Insert fittings only seems
to work with content center items, parametric or dumb all the same. If you
don’t know what I just said I suggest you get familiar with my blog on
inserting fittings here.
Placing fittings
will insert nodes on the route which breaks constraints and remove dimensions.
A better way would be to place the main fitting say a valve and insert the rest
of the fittings before and after, like reducers, unions, etc. This way you only
need to control the position of one node on the route and the sketch remains
fully constrained. Insert fittings only works with content center items and to
overcome this you would first need to place a CC item and then drop your
library item (located on disk) over that CC item. These are way to many steps,
so for this we will publish them to CC as a family.
I am going to
use a Georg Fischer valve set as an example.
TIP: You can download the whole Georg Fischer cad files as zipped
packages split by material type, ABS, PVC-U, PVDF, etc.
Georg Fischer metering valve as example.
I needed a
metering Valve so, to replicate my case, after locating the stp files start a new assembly in
Inventor. Drag the step files inside the graphical window of the new assembly.
If the files are computer generated then the origin will match for every single
one of them even though when they are dropped in the assembly they will be automatically positioned at certain distance from one another. You need to position them on a common origin, and even better to
the origin of the assembly. Use the Assemble tab, Productivity pane, Ground and
Root Component command to fix them at the origin really quick. As you can see
in the screenshot I have GR as my speed key and that helps a lot.
TIP: The files will be imported as per the last Options you chose for this particular foreign file extension. If they are being imported as composite surfaces rather than parts with bodies read down towards the end how to change the import options.
Use Ground and Root Component to fix them at origin.
This is a
perfect example because with 2 models we are going to cover 4 members in
content center. Because the models are the same there is no point getting all 4
stp files and only 2 will do. The other 2 models are identical having different part
number due to different gasket materials.
If the models
had a common origin you should see them overlapping just like on my section in
the image bellow. If not you will have to constrain them to a common origin,
and then to the assembly origin.
Locate imports on a common assembly origin.
The next step is
to get this assembly as a single multi-body part because for now it’s only
parts that can be authored as T&P and parts only that can be published to
CC. Derive and Shwrinkwrap didn’t worked in all my tests because the bodies
were not coming in as suppressible features. Save the assembly as “stp” because
“sat” for all my tests looses the color of the bodies and I don’t want to fix
appearances as well. Click open and browse to the new stp. location. You might need to change the file extension
filter to Step or Any (*) and select your file. Click Options next to Open and
then make sure you choose Solids, Assembly as Single Part and Multiple Solid
Part. This will allow you to suppress the bodies unlike doing a shrinkwrap or
derive.
Shrinkwrap or Derive didn't worked for me.
Use the Options button before Opening the document.
TIP: If you don't get solid bodies on your imports you can play with stitch, sculpt, combine, and get solids out of surface bodies, but we do need bodies for the suppress command.
In the part
environment use Parameters and add two parameters, z and L (my case) which will
be your connection distance and engagement distance. For butt weld you don’t
need an engagement distance. Just like in authoring empty parts we will create
work points for our connection reference using work planes located at L/2 on
each side and the inline origin axis. As you can see the catalog has no
dimensions for z but I have measured the models and added the value to the
table.
Missing dimensions can be measured on imported models.
Create connection points using parameters.
Before you click
the create ipart button I suggest you rename the bodies in the browser because
they will be hard to identify on the ipart table. Here’s my example, and
remember that a single body will serve 2 family members. If you don’t do this,
in the ipart table you will see “body1”, “body2”, etc. which is hard to locate.
Rename bodies to make easier to identify in the ipart table.
Once finished
adding the ipart table info test the model by switching between ipart members
and see if the model updates. I have an excel spreadsheet as template for Georg
Fischer families and once I’ve clicked on create ipart, I close the table without edits and I open it in excel where it's easier to paste the
data from my template which covers, material, description, DN, part number,
etc.. and even cost and stock info.
Test your model by switching between components.
Author the ipart
as Tube and Pipe component using the connection points created and the “To
Plane / Point” option choosing the engagement planes.
Author and publish your part to Content Center
Once you publish
this to Content Center you have access to Change Size command but most
important the Insert Fitting command.
Insert Fitting is working for CC items.
Keep in mind
that adding all these bodies will increase the size of the file a lot and for
simple parts you are better off to model it rather than adding them as
suppressed bodies which can be a bit of overkill.
Hope you are
still with me; I will do a video for this might seem too much to some of you.
For your
convenience I have attached the files in a zip document so grab
it here and start playing with it.
This
was really scheduled to go out on Friday but I was just given a major-major
project with strict deadlines and huge penalties on our side for any delay so I
had to put in the extra hours and effort to get it moving. I hope I haven’t
ruined your weekend by giving you nothing to read on your Sunday coffee or
whenever it is that you catch up with the past week news, blogs, forums and CAD
news altogether. Helps to start work with a bit of laugh and irony.
Part two on
publishing dumb parts is all about authoring empty parts. A lot of the times
you don’t have the final model because it’s a complicated part to model, you
don’t have enough time or information, you are waiting for a different department
to model and certify the part. So meanwhile you do as best you can to overcome
this, constraining and moving components around to account for the missing elements.
Empty on all sides
You
might take it a step forward and create a similar shape body or surface outline
to guide you as of what the occupied volume is so you can avoid any clashes and
interferences when the final model will come in place. This applies to everything
from valves to skids and other equipment like heat exchangers for which a model
doesn’t exist and it’s in the process of being finalized.
When I am
dealing with this type of situations I usually create an empty part, author it
as Tube and Pipe to serve me in my routing and drop the final model when ready
over it with place fitting command.
TIP: The he assembly replace command will not work and
you need to use place fitting instead. With the place fitting command you can
drop any T&P authored part on top of a different one to create a replace.
In
my last post here,
I’ve shown you how to better/faster create work features and if you haven’t
seen it go check it out and then quickly come back because we are going to use
that same techniques here.
In
order to author a T&P fitting you need a work point for the connection and
an axis for the direction of the engagement. You might need another plane to
setup the engagement distance but that depends on the type of connection.
You
probably did these points instinctually when authoring T&P fittings although
you don’t need to. On an empty part you can’t do without work features but on a
model with circular edges you don’t need any work features at all; will have
to detail this at a different time.
If
you can’t use the origin planes and axes then you need to create your custom
work features and I recommend that you rename then work features in the browser
to help you find them on later edits.
TIP: If the directional axis matches one of the origin
axis then you don’t need to create them AT ALL. The directional axis doesn’t
need to be in line (coincident) with the work point and here’s to prove that:
Add caption
I know there’s nothing fancy here but a lot of people are unaware that
you can author empty parts and it’s really the foundation for authoring dumb
parts as we will discuss next time.
Still buried
with work and not sure if I’ll be able to do a video but at least you will have
some quick info on how to do but fusion fittings and routes in general.
Depending on the complexity and detail you need there are a couple of
approaches to take here. The simplest one would be to ignore the discrepancies before
and after the pipe welding but you can take it all the way and create your
excess welding material as ifeatures that you can drop on each fitting you
author.
On my plant
layouts I always ignore them because we tend to have plenty of space and discrepancies
can be ignored. Quite simply on a 10 meter pipe the assemble tolerance will
incorporate any variation from welding or thermal expansion.
So unless you’re
into designing medical equipment or any other precise, tight tolerances
equipment I would not bother. Keep this as a reference if every once in while
you need to do renderings, or the client asks for these welds to be in place
and ignore them the rest of the time.
On the simple
side, quick and dirty if you do need to have proper, exact cut-to-length dimensions
and BOM reports then you need to over-define your engagement dimensions so that
the parts interfere therefore reporting correct pipe length and correct route dimensions,
node to node.
If you do need
to get all that detail exact and you have all the time in the world I would
suggest you do the fusion as a ifeature that you can drop on each fitting. Make
that ifeature table driven so you can choose and change size on the fly. You
can take it down another level and calculate the lost volume from the cutout
(melting) and generate your weld bead based on that but that’s way too granular
for me.
If you need to
author ipart fittings like elbows, tees, or anything else that has a table and might
go to Content Center then define new planes driven by the fusion distance and
set your engagement to plane/point so you can drive the engagement for each
fitting diameter separately.
I recommend that
you don’t change or re-author the pipe because you might use that pipe on
different connection style (socket welding, jointed, etc.) and it will mess
those up. Do all these changes on fittings and it will drive the pipe
engagement as well.
On my last post
I’ve shown you how to place fittings when in a hurry and as promised, today I
am going to cover pipe clips, hangers or vibration mounts.
I’ve got a
really nice trick on how to author them so that you can drop them as T&P fittings
and yet have BOM reporting full length pipes. As we will see we can control the
position of the clamp with a node on the route but the pipe will not be
interrupted and report a full length.
In order to
create the ipart and Content Center Family I’ve downloaded the PDF catalog from
Georg Fischer but just like all catalogs it doesn’t have all the necessary info
to build your 3d model and family table so I had to download the step files as
well. Just to try out and for fun I’ve downloaded the
feature recognition tool from Autodesk Exchange App and decided to use it
to transform my step files into feature populated Inventor file. This is on
subscription only but you don’t really need it, because you can open measure or
project your step file.
As soon as you
open a foreign part it asks you if you want to recognize features and it will
open a new environment where you can choose the type of features you want to
identify. You need to make your way backwards starting with chamfers, fillets,
holes, and then revolved and extruded features. Each recognized feature will be
hidden from the model and as soon as you identify the last one and you exit the
environment you will have all the features in the browser.
So after
measuring all the step files for missing dimensions and building my table I was
ready for authoring it.
How do you author this without interrupting the pipe when the node
gets created?
Drum roll please……
You need to author it as “Branch
Fitting”. I thought about this solution long ago when I’ve done a branch
fitting but didn’t got enough time to play with it and I am pleased to say that
it works just as expected.
If you don’t know what Branch fittings are or you don’t know how to
author them please take a look at my blog here.
They should look like this:
In the Tube and
Piepe Authoring dialog you need to provide the following information as a
minimum:
1 – Type: Branches
2 – Connections:
at least one and in the case of the clamps that will be enough
3 – End
treatment: Joined. This is up to you on what you want to specify, I tend to use
joined mostly. Habit of not having the T&P styles complain about different
end treatments.
4 – Minimum,
Maximum Nominal Size: ND (from ipart table). This is because a pipe clip as a
branch fitting can accommodate several pipe diameters but I’ve only done a clip
each pipe diameter.
5 – Mating
Point. You need to create this point, easiest would be to have it in the pipe extrusion
cut sketch tangent with the pipe circle vertical with the pipe center at the
bottom (check down below more info on this).
6 – Pipe Axis.
You can click on a cylindrical face of the clamp (concentric with the pipe), or
choose the origin axis (if your part was properly defined) or create your axis
before authoring. The pipe will not always go through this axis, check bellow
more info.
7 – Cut Mating
Pipe. Normally on a branch fitting I would say yes but in this case we don’t
have a cutting sketch defined and we don’t need the pipe to be shown with a cut where the clip is.
TIP: Once you finis authoring
and you get success after clicking ok you might be surprised to find that the
authored info does not persists. If you try to author it again the pie axis
moves to the mating point and now it fails with an error. “The selected
mating point and pipe axis are collinear, please select again.”. This is a
bug, don’t let it stop you, author it again and carry on, publish to content
center or save it to your library, it will work so re-select and fix the axis
and point info and continue.
The
pipe axis although defined I can’t see it having too much importance; except to
be used as a direction reference for the pipe in regards to the mating point.
The mating point is where the pipe will connect; outside face of the pipe
coincident with the mating point ending up with a sort of tangent constrain
between the pipe and the clip. This makes sense because the pipe looks like it’s
sitting on the clip.
I suggest that
you ad custom parameters for your pipe clips to help you place and dimension
the node. I have two parameters, one for clip thickness and one for clip
height. The clip thickness helps me dimension the node in regards to existing
nodes and included geometry. In the image bellow I have an elbow followed by a
pipe clip and with a gap in between, so the dimension becomes: e + cp + gp.
Clip
height I use to dimension my route from walls, floors and mounting surfaces.
I import my
parameters every time when starting a route.
You don’t need
to do it this way, you can position the clip (node) when placing the fitting.
As soon as you drop it on a pipe and you get the rotation arrows you can right
click, select Point Snap and type a distance while holding the mouse over a
face. It will position the node at the typed distance from the face where your
mouse was positioned.
Try this out, it’s
really nice and it’s working for placed fittings as well, just choose Edit
Fitting Orientation (need to be in the run) and then activate point snap. It
doesn’t create a dimension for the node and I recommend that manually dimension
it just to stop the segments from flying around and get your route in the “Violation
Mode”. Try and keep the sketch fully constrained as much as possible.
That’s nice and
seems to be working pretty good for iparts and CC items but what about custom
length stud mounts, where I need a different dimension all the time and
sometimes I don’t need the end nuts because I am welding the stud to my skid
frame.
Unfortunately this
bug persists in 2016 beta as well so you can’t place T&P authored iparts or
illogic components. The work around is to open another inventor session where
you disable your T&P add-in and you generate your files there then place
them in and Inventor session that has T&P enabled. This is tedious and time
consuming, not to mention that you can’t control the file name, part number and
properties of the component and it places it next to your assembly instead of
having it in the library.
When you place
an ilogc part the select size and configuration menu appears but as soon as you
accept your info Inventor reverts back to “select fitting to place” dialog
instead of creating and placing the customized part.
iParts are even
worse, for they don’t even ask you for the parameters to change, it just drops
the main file into your assembly.
Hopefully they
take our posts on the Idea Station seriously and if you haven’t, I suggest you
go give us a vote to improve T&P module where I’ve got around 50
bugs and improvements on one post here:
Luckally until Autodesk
fixes this I have a solution and that would be to use Multi File Manager
(MFManager formerly mExtension) that I have so widely covered on my blog. Do a
search on my blog if you don’t know what mExtension is.
On the place
menu of the Assembly tab there is a new entry called “Place From Libraries” and
it looks very much like the search window where you can search for files on
disk. In this case you search for the file to place.
1 – Place from
Libraries
2 – Put * in the
Name or leave it blank to search all
3 – Select the
file type you’re searching for
4 – Select the
path (.. . to browse or down arrow to choose from last used locations). Don’t
search subfolders.
5 – Search
6 – Select the
part you want. Icon with a table shows iparts while one with fx will be illogic
components.
7 – Insert, to
place it in the libraries or Insert Local to place it next to your assembly in
the workspace.
The customize
part dialog looks just similar to the one on place illogic component but you
get the description of the key parameter as well to better understand what you’re
changing and you can see all parameters not just the ones marked as “Key”.
As soon as you
drop finish customizing and you click apply the fitting can be dropped anywhere
on an existing node or on a pipe segment and it’s nicely positioned in the run
not just anywhere so you can use this from anywhere like being on top level
assembly.
Several users have reported that while you can author a branch fitting with a single connection, Inventor fails to place the fitting.
I have posted the solution on Autodesk Forum as well (see >>this<<) but here is the explanation. For some reason if you start with a blank file from templates, having
a single connection doesn't work. If you, however, start by stripping
down an existing branch fitting from ContentCenter (like a weldoled)
then it works. You can also use my files from the blog, down at the end. Open your current file and my clip, delete all features from my file,
copy all the features from your cfile and paste them into mine. Continue
authoring the file, optionally you can publish it to content center,
and test it.
I haven’t
finished with all the tube and pipe posts, just got sidetracked with authoring
fittings and decided to share the problems and solutions found along the way.
Can’t remember
if this has always been a problem but in 2015 even though you follow all the
known steps and procedures you don’t always end up with usable tube and pipe
fittings. I have been publishing a couple of fittings for a new route style and I found that you either end up crashing inventor or they can’t be
found while browsing on the new T&P (tube and pipe) style dialogue.
First thing I
recommend is to check the pipe and fittings end treatment. In my case the same
pipe can be but welded or socket welded while the fittings (elbows, tees) can
only be socket welded or but welded. So I used jointed on the pipe and jointed
on the fittings no matter what type of connections they really are. On the
fittings use different engagement distances to differentiate between socket and
but welding. This is to avoid warning message every time you edit the style
about non matching end treatment connections. Remember I don't keep any styles inside the T&P template but import the ones needed when starting a new T&P assembly.
We don’t use
ISOGEN exports but I like to have it setup just in case we will ever need to.
In my ipart table I have setup ITEM-CODE and ITEM_Description columns that I
have used in the tube and pipe authoring dialog. The only column that needs to
be on the ipart table is ND (nominal diameter) that I use as key when
publishing to content center and that Inventor uses in the tube and pipe style
setup. You can add this column while editing the ipart in the custom tab or you
add it while editing the ipart table with excel. I like excel because it can
contain any information you can think of without messing the ipart table. As
long as you leave an empty column (actually first cell of a column) between the
info you want in the ipart and the rest of your data, you can have any info you
like. Formulas, graphs, images, even catalog pages from the manufacturer.
Setup the ISOGEN
properties and engagement correctly but leave the end treatment to jointed.I don’t have a shoulder for pipe limit stop but I have created planes
that will serve as my engagement limit in the author dialog.
You need to understand that socket and but weld “End Treatment” filter
on the library browser while setting up you style, will not get you these
parts; “jointed” will. So don’t filter by socket or but weld, as you will see
later I use Standard and maybe Material as my filters.
After you finish publishing to content center you will find that a “Designation” column is added
automatically by Inventor and it’s linked to the part’s “Design Tracking Properties: Size Designation” which is of type
string and can be edited but not in the iproperties window (code or else).
It seems this is used only for content center
stored parts and represents a “succinct
user-friendly universal way of providing a name for the component represented
by a row in the table”. This is copied from an old pdf I found on
iproperties and VBA by Sean Dotson at AU2014. Most of the times you will have a
description of the item like “d10 x 1 – 250 Lg” and it doesn’t need to be
unique. I think this has been left over and obsolete so I would just ignore it except when it gives you problems with tube
and pipe style as it did to me.
It seems that it can be accessed
as “Content Library Component Properties” as well:
Comments: Size Designation: String (VT)BSTR),
Editable, No UI, Succinct, user-friendly and universal way of providing a name
for the component represented by a row in the table.
Why have I gone
to such length and dig out old posts and manuals to find the info on
Designation? Because I found it to be the source to my problems, and there’s no
logic to what my problem is as well.
I've been having
this weird problem with tube and pipe styles. After I author and publish a tube
and pipe fitting it won't show up for selection in tube and pipe styles until I
edit the family table and delete the
designation values. I don’t edit the column formula just select all values
in this cell and delete them. Because the column is an expression
the cells update automatically to same values but now the family
appears in tube and pipe style editor.
As soon as I delete the designation
values, the family appears in the styles editor as you can see in the animation
bellow, where I have 2 inventor sessions running at the same time.
In the style
component browser if you expand your part you will see individual members as long as you have a unique individual
stock number. The members are shown by stock number and AU explanation was
that part number can have custom lengths so not suitable to use here. I don’t
pick individual components just the family when setting up the styles.
Hope you never
run into these problems but if you do try deleting the designation values and
see if it fixes it. Next week I will
share a couple of excel tricks for retrieving data from other spreadsheets with
vlookup match and error handling like when value not found returning #NA so
check back. Hopefully I will finish the rest of Tube and Pipe tutorials. I will also share this elbow and excel as separate file (it's embedded anyway in the ipart).
