Digital simulation of a patient lift

Out of category
1

Hi all!
I was in charge of designing a patient lift, so in order for me to do the design I find problems in terms of numerical simulation; where the connectors!
Well, for the system is simple; with the help of an electric actuator that will push the arrow to the place where the patient is held with a flail.
The ambiguity lies in the connections between different parts where some parts are fixed (bolted and welded) and others are hinged.
Attached is the structure of this lift.

Kind regards 


fig1.png
2

Hi @ firasschafai

In my humble opinion your charging point is badly placed 

It should optimize stability 

to be as close as possible to the center of your 4 wheels

imagine putting a mass of 100 kg or +

Hanging at the end of your arm 

For sure the whole thing dives the nose

@+

PS: see this link among others

https://www.handimove.fr/produits/leve-personne-actif

3

Good evening @ gt22 
I totally agree with you.

but I direct my question to the type of connections, because I tried but every day the results are huge!! we are talking about a safety factor of about 0.4 !.
So I think I chose the connections wrong!!

4

Hello @firasschafal

If we are talking about a simulation made with Solidworks simulation then we just have to put a bearing load connector or simpler a simple load on the axle at the end of the stem. In the case of the load do not forget to designate the direction of the mass.

Be careful, before doing the simulation, you have to remove all the bolts, the casters, etc...
Then create two zones with dividing lines. These areas can be the flat areas or would be fixed the casters according to your drawing.

Do a check with the "collision detection" tool otherwise your simulation will fail.

For the safety factor you need at least 2 and rather 3 or more (disabled people do not need additional problems).

But first of all , since you already seem to have results , you should send your file with the Pack and go function and imperatively attaching the result of your simulation and all in a ZIP file. From there I would look at what is going well and what needs to be improved. Otherwise, we risk speaking in a vacuum.

Kind regards

2 Likes
5

Hello@gt22

The connectors @firasschafal  are talking about are the ones used in SW simulation. They don't have much to do with bolts.

A little tease on my part ;-) The lift you show is closer to a sit-to-stand while @firasschafal wants to make a bariatric lift which is very useful for weighing the person, bathing or transferring them, etc...  https://andreviger.com/fr/leve-personne/313-leve-personnes-bariatrique-rpl-600.html

As you point out in the background, you have to target the maximum weight because for bariatric the sizing of the sections is more substantial. What you point out about the position of the CG in relation to the tipping point is very relevant, it is obviously obvious. There are other elements that don't go AMHA in the design, but I'm just answering the "SW simulation"  question; -)

Kind regards

1 Like
6

Hi @ Zozo 

You also have the right to search on the link I posted 

there are several models ;-)...

and it was only for the example that allows you to visualize the ref points

have a nice day @+

1 Like
7

Hello @Zozo_mp
It's my return with you!!
Well, I now find a CS=0.27!! really it's nonsense.

I totally failed to solve this problem. Indeed, the problems here are that I chose the connectors badly, and despite the fact that I did the loading as you proposed with a loading on an axis (with the  direction).

Well, for the structure I made there is a trick at the bottom is that the legs will be foldable by using the lift, in other words a pivotal connection between the two parts of the feet.
So, I'm sharing the zip file with you to head to a good CS. 

Kind regards 


leve-personne_sw.zip
1 Like
8

Hello

Hello Houston we have a problem!!

Apparently you have a version of SW higher than the 2019 (future version) which means that I can't do anything with your files.

Simulation of my version is not compatible.

However, a close look at your image shows several things that are wrong.

1°) For me, as your model is, you have a coefficient of 2.7.

2°) The current coeff is not good anyway because your model is not correct at all.

3°) Your way of proceeding for your fixed points is wrong

4°) your cylinder is missing, which means that the stem effect (bracing) of it does not work.

5°) you use the beam mode instead of using volume. The beam mode is a source of trouble if you don't master it completely. You mix solid parts with beams, which complicates your task without adding more.

6°) You have too many interpenetrations (I have counted at least 12) which is not possible in real life. Normally the mesh should fail with a message indicating the number of interpenetrations. The result of the simulation is normally completely wrong as a result.

7°) it will be necessary to use a remote load to take into account the modification of the Center of Gravity (the center of mass) if the lift is moved on a slope, even a slight one.

8°) You will have to independently test your connection which is used to bend the feet. Which, by the way, cannot be folded up as it is without dismantling a through bolt and without having a rotation axis.

Explanation:

Your model should touch the ground, it's what you do with your fixed points at the bottom (in green).
I note that they are overcrowded and therefore useless. But more seriously, you put fixed points in place of the cylinder clevis and the axis of the cylinder rod. This makes your simulation look as if the rooms were fixed in the wall or a virtual room. As a result, you cannot have the correct stem flexions or load descents.

Tentative conclusion:
All the mistakes must be corrected before going any further.
 

Courtesy remark: A Mon Humble Avis when you have done your simulation it will reveal the defects which are of what I see already prohibitive (without the simulation).

You shouldn't want to go too fast in design and pay attention to all the details.

Kind regards

1 Like
9

Good evening @ Zozo_mp

A lot of remark means a lot of problems!!

Can I send you the coins with the IGS format?
Well, I tried again with as you told me with remote mass loading, but everything will be unitile when the simulation is done on mixed parts between volume parts, and membranes.
Well, for interpenetrations I have already checked the parcels but the result gives "zero"!
Essentially, and too quickly I get to know that I have to change the  whole structure into volume parts, so I rebuild the profiles as well as the folded parts, that is the first step, and then the seat of the connections!! The conditions of which are the limits of the fixing at the end of the castor holders (on the ground), bolt-type connections between the two parts of the legs (it is really the pivot axis or the case of being foldable), between the Mast and the jib is the rotation axis (up and down mode of the stem).



Good for the cylinder, I just applied the fixed pivot to the axes of the cylinder attachments (one on the Mast fixes the cylinder and the other on the jib to fix the cylinder axis) so I think the presence of the cylinder is useless! No!.

Kind regards 
 


boulon1.png
10

Hello @firasschafal 

You need to put the cylinder even simplified because it is the one that will measure the elasticity.

You have to convert all the pieces, into volume pieces without exception, it will be simpler.

There is no need for bolt connectors or casters for your set, I understood your assembly very well (and especially your folding legs). I can view your entire model but I can't use it to make a simulation

By taking into account my previous remarks and adding the cylinder, you will be able to make a first simulation to rough up the subject.
However, it would be desirable to integrate @GT22 's remarks beforehand, which I welcome in passing!

We will see afterwards, and only if you wish, on what will cause you problems in my experience. Problems that can be confirmed (proven)  by a more targeted simulation in a second step.

Kind regards
PS: I hope you're doing well  ;-)

11

Hello @ Zozo_mp

Ooh la la !! I'm going to shorten the model to a simpler model, simulate it on the stem, the mast and the addition of the cylinder because really I failed several times with the results.

I'm totally in " burn out" and my pc uses 11Gb of RAM on a simulation of a lift...
Time flies too fast and I'm lost on this simulation.
Well, for the simplified model I find a result that can be said "catastrophic"  


 
For the connections: I put a fixed support at the bottom, a fixed pivot at the level of the joint between the jib and the mast, as well as at the level of the cylinder.
The cylinder is rigid.
We have to boost towards the better. 

PS: to you too, I hope you are doing well Corona.

Kind regards 

12

Hello @ Zozo_mp

A return with you!
Another try, and hopefully all is well with 2.4 CS and 1.4mm displacement.
It seems a bit logical to me, if the boundary conditions are fair.

 

Kind regards 

13

Hello @firasschafal 

Sorry!!!    but your simulation is not good at all because you don't take the right settings.

Here's what you should get instead. If you want the ASM to be able to transpose on your model I am in SW 2019 SP5 so usable in 2020 version.

@tous The model is fanciful but it only serves to indicate all the parameters necessary to achieve the desired  result ;-)   ;-)

Kind regards


leve_personne_-_principes_pour_la_simulation_-_2020-08-26_14_51_16-window.jpg
1 Like
14

Hello @  Zozo_mp

It's great really!!

Frankly, I can't argue about the results because as an engineering student in the final class of mechanical engineering I have practically no professional experience except for the achievements in internships.

Closing the subject, I totally agree with your result, so I can take your ASM because I use SW 2020.

Thank you so much.
Every day you are the Saviour !!

Kind regards 

1 Like
15

 @firasschafal

Take a good look at the different constraints that I put in the model.

1°) I made a delimited area to fix the part where the mast is. This limited area corresponds more or less to the support area of the caster which does not need to be modelled.

2°) On the other hand, with also delimited areas, I put a flat support which would allow, if there was a big deformation, these areas to move away (or move) from the other wheels. It is not visible to the naked eye, but in the event of deformation, the castors on the right move slightly away from those on the left. (to be confirmed with your 2020 model)

3°) Then you have to put pin connectors in the three holes (clevis and cylinder rod) and then at the place of the mini beam joint. All bores must be selected for a hole (four in total per hole). You will see that then SW creates a fictitious axis but which contains all the information for the simulation. This type of axis simplifies the mesh, which consequently has a shorter execution time. For these axes, select circlips and keys to immobilize the axis. (it would be possible instead to use "fixed pivot" which eliminates the radial and axial translations).

4°) I put the vertical load with a vertical reference frame located on the foot. So even ^me if the beam were to bend by deformation the direction of the load would still be vertical (very important) I could have put a ring and put the load on the ring but it would not have added anything except unnecessarily complicate the whole)

Last point: use the "animate" function in the result area you will see in real time how the deformations are made. (animating only works for "Von Mises" and "Move"

Kind regards

 


leve_personne__zz_v1a.zip
2 Likes
16

Hello @ Zozo_mp 

The most careful thing here is that the maximum stress is in the Mast (at the bottom)!
So the optimization of the design, including the addition of a base for example, or any reinforcement is necessary ( now it's my task ;-) ).

Well, if we imagine the contrariant will influence the jib more strongly than the Mast, so the buckling of the cylinder, but it is better to direct the maximum stress on the Mast, because on this we can change it by reinforcements unlike the jib.

The connectors are very explanatory and reasonable.

It's time for me to have fun with animations ;-)

Kind regards